论坛 › MSC系列软件专区 › [共享］The MSC＿PATRAN FAQ转自剑桥工学院

stuartgew 发表于 2006-6-13 16:59

[共享］The MSC＿PATRAN FAQ转自剑桥工学院

关于patran的基本问题，有详细的解释
很不错的说
需要的可以看下啊


The MSC/PATRAN FAQ
________________________________________
1. General Questions
Q1.1 : How much disk space do I need?
Minimum of 10 MBytes. Probably about 20 MBytes for medium sized problems. The patran database can be typically 2-3 MBytes in size. In order to compact a patran database which has grown in size 8 to MBytes you would require 8 MBytes of free disk space in your HOME directory. This is because patran makes a backup copy before compacting it. Compact should not be confused with the unix command compress. This command can be used to save disk space if the patran database is not going to be used for a while. Use the unix command uncompress before accessing a compressed database next time.
Free disk space is not required to use the compress command. The compressed files have the extension .Z added to the file name. For example if you have a database called earthquake1.db the compressed file will be called earthquake1.db.Z.
________________________________________
Q1.2 : What finite element analysis modules are available ?
ABAQUS and P3/FEA are available in the teaching system.
________________________________________
Q1.3 : What type of analysis can I do ?
It depends, if using ABAQUS the following solution types are available :
Click on radio button Analysis and in the form select Step Creation.... In the new form look at the Solution Type.
•        Linear Static
•        Natural Frequency
•        Bifurcation Buckling
•        Direct Linear Transient
•        Direct Steady State Dynamics
•        Modal Linear Transient
•        Modal Steady State Dynamics
•        Response Spectrum
•        Random Vibration
•        Nonlinear Static
•        Nonlinear Transient Dynamic
•        Creep
•        Viscoelastic (Time Domain)
•        Viscoelastic (Frequency Domain)
These correspond to the ABAQUS procedures listed below (in alphabetical order) :
•        BUCKLE
•        COUPLED TEMPERATURE-DISPLACEMENT (steady state and transient)
•        COUPLED THERMAL-ELECTRICAL (steady state and transient)
•        DYNAMIC
•        FREQUENCY
•        GEOSTATIC
•        HEAT TRANSFER (steady state and transient)
•        MASS DIFFUSION (steady state and transient)
•        MODAL DYNAMIC
•        RANDOM RESPONSE
•        RESPONSE SPECTRUM
•        SOILS, CONSOLIDATION
•        SOILS, STEADY STATE
•        STATIC
•        STEADY STATE DYNAMICS
•        VISCO
If using P3/FEA the following options are available.
Click on radio button Analysis and in the form select Solution Type.... In the new form look at the Solution Types available and choose one.
•        STATIC
•        MODAL
•        BIFURCATION BUCKLING
•        NONLINEAR STATIC
•        DIRECT LINEAR TRANSIENT
•        MODAL LINEAR TRANSIENT
•        FREQUENCY RESPONSE
•        SHOCK SPECTRUM
•        DESIGN SENSITIVITY
If you are interested in thermal analysis then click on top menu Preference and choose Analysis.... In the new form change the Analysis Type : from structural to thermal. Click on the OK button in that form.
Click on radio button Analysis and in the form select Solution Type.... In the new form look at the Solution Type and the following option should be available.
•        STEADY STATE HEAT TRANSFER
________________________________________
Q1.4 : What output options (including hard copy) are there ?
The following hard copy options are available :
1.        Colour postscript (A0 to A4 size).
2.        hpgl (A0 to A4 size).
Choose File from the pull-down menu and then Print.... In the new form choose either postscript or HPGL for the driver and then click on Page Setup .... In the new form choose the appropriate Paper Size. Example A4. Then click on OK.
In the original form click on Options ....
If HPGL option has been selected then in the new form
click on Print to File (square button). Click on OK in this form and in the original form click on Apply.
If Postscript had been selected then in the new form
click on Print to File (radio button) if you want to create a postscript file. Click on Create EPS file (radio button) if you want to create an encapsulated postscript file.
If you want to send the postscript plot direct to the plotter leave both these options unset.
Finally click on OK in this form and in the original form click on Apply.
Create eps (encapsulated postscript) output file if you want to include it in latex documents (reports/thesis).
________________________________________
Q1.5 : Can I import the geometry from elsewhere ?
Yes. If the geometry was generated in Pro/Engineer then this data can be transferred directly to Patran.
If the geometry was generated using some other CAD package then the data can be transferred using an IGES file. However be prepared for unpleasant surprises. Lines, surfaces may go missing if you use this option.
In PATRAN one of the example problems demonstrates the importing of an IGES format file.
Choose Help from the top menu and choose Document Library... Select Part 10 : Example Problems. The Example 2 : L-Shaped Bracket illustrates the use of importing a IGES format file. The install_directory is /export/msc/patran8/patran80 ie the IGES file is /export/msc/patran8/patran80/test_files/bracket.igs.
To run this example first copy the above file to the directory from which you are running Patran from.
Choose File from the pull-down menu and then Import.... In the new form change the source from Neutral to IGES.
The IGES format file should be given the extension igs (Example : bracket.igs) and should appear in the list of Neutral Files. Select the appropriate file and click on Apply.
If you want to check how successful the reading of the IGES file was click on IGES Options... in the `import' form. In the new form click on Preview IGES File.... This will bring up the Preview IGES File form. Click on Write to report file and then select the IGES file and click on Apply. Then you can look at the report file and see what information had been successfully read from the IGES file.
________________________________________
Q1.6 : Can I import the f.e.mesh from elsewhere ?
Yes. If the finite element mesh data (nodal co-ordinates, element-nodal connectivity list) is written in the Patran 2.5 neutral file format. See the section 11.2.2 for the Patran 2.5 neutral file format. For example if you have used the DUCT program to create a surface and then meshed it the finite element mesh data is first written out to a file. Then run the duct2pat conversion program which writes the data out in Patran 2.5 neutral file format. This file can then be imported into Patran.
Choose File and then Import.... In the new form object should be Model and the source should be Neutral. Click on the Neutral Options ... and in the new form the heading Entity Packets lists the entities that can be read form the neutral format file. Click on OK in that form.
The Patran 2.5 neutral format file should be given the extension out (Example : bracket.out) and should appear in the list of Neutral Files. Select the appropriate file and click on Apply.
________________________________________
Q1.7 : Can I import a IGES format file ?
Yes. See the answer to question 1.5 above.
Choose File and then Import.... In the new form object should be Model and the source should be IGES. If the source is Neutral then change this to IGES.
Click on the IGES Options ... and in the new form the heading Entity Packets lists the entities that can be read form the IGES format file. Click on OK in that form.
The IGES format file should be given the extension igs (Example : bracket.igs) and should appear in the list of Neutral Files. Select the appropriate file and click on Apply.
________________________________________
Q1.8 : Can I export the f.e. mesh data ?
Yes. You can write out the finite element mesh data in the patran 2.5 neutral format.
Choose File and then Export.... In the new form the format should be Neutral. Click on the Neutral Options ... and in the new form the heading Entity Packets lists the entities that can be written to the neutral format file.
If you are only interested in the finite element mesh data then highlight only the following :
•        Nodes
•        Elements
•        Material Properties
•        Element Properties.
Ensure that for Existing Groups the group which contains the finite element mesh is highlighted. Then click on OK in that form.
In the original form enter a name in the box marked Create New File and give it an extension out. Example plate.out. Then click on Apply.
________________________________________
2. Files/Databases
Q2.1 : After running PATRAN I have several files created in my home directory. Which files do I keep?
You need to keep the following files :
*.db,    *.db.jou

Example : plate1.db,plate1.db.jou
These are the essential files. First is the patran database. The second is the journal file which can be used to re-create the database in most cases.
The following session files can also be kept. These can be used to run demos.
patran.ses.*
The following are the patran message files :
*.msg.*
Unlike a single journal file there are one session file per patran session. The following are the additional ABAQUS files :
*.inp
*.msg
*.dat
*.fil
*.log
*.com
None of the ABAQUS files need to be kept.
________________________________________
Q2.2 : Have set up the f.e. data. Ran the ABAQUS analysis. No errors reported in the *.msg.* file. However the *.fil does not show up under the list of "Results File" on the "Read Results" form. What do I do?
In the odd instant even if the *.fil exists it may not show up under the list of "Results File" on the "Read Results" form when you click on the filter button.
To check use a separate X-term window and go to the directory from which you are running patran from (this is listed in the top of the "Read Results" form. Type ls -l *.fil and this will list all the files with the extension fil in that directory. If the *.fil file exists then go back to Patran and click on the "filter" button again. If it does not list the *.fil file in question then type in the fil file name (including the full path name) in the box marked "Selected Results File" and click on the "OK" button. This hopefully should read the results from that *.fil file.
________________________________________
Q2.3 : After creating a separate directory for running Patran, I can't find any of the Patran files in that directory?
In the "Open/New Database" form it is possible to move to directories other than from which Patran was invoked/started (using the filter box). If you had not invoked Patran from that directory then the Patran files will not be placed in that directory.
For example if you are a first time user you may have a created a separate directory but forgetting to change to that directory before invoking Patran is a common mistake.
Go to your HOME directory using cd and then use the following command to search for the patran database.
find ./ -name "*.db"
The other Patran files will be found in the directory from which you invoked PATRAN. If necessary move these files to the desired directory using the mv command (make sure you are NOT running PATRAN while you are doing this).
________________________________________
Q2.4 : I have accidentally deleted the patran database (*.db) or it appears to be corrupted. What do I do?
First contact the computer operators (oper@eng.cam.ac.uk) to see whether it can be recovered from backup. This is the recommended choice.
If not you can use the corresponding journal file *.db.jou to re-build the database. For example if you have deleted the database plate1.db then look for the plate1.db.jou. If this file exists then start patran and then choose File / Utilities / Rebuild... and then choose the plate1.db.jou file and click on OK. This should re-create the database in most cases.
If the plate1.db.jou does not exist then you could try using the patran.ses.* file. This time choose File / Session / Play... and then choose the patran.ses.* file and click on OK. This is more likely to work if there was a single session file for the *.db in question ie all the work in creating the database was done in a single patran session.
If the work was carried out in several patran sessions then there will be one session file per session. Then these session files after minor edits to remove opening and closing of the said database can be run is sequence. However this method is frought with problems and the re-creation of the database may not be completely successful.
________________________________________
Q2.5 : The patran database I was using has grown into several Megabytes in size. What do I do?
First check the size of the Patran database (using ls -l *.db ). If at least the same amount of free disk space (use the quota or du command) is available then choose File / Utilities / Compact... and then choose the database. Then click on the OK button.
If not then you have to move the database into a temporary directory. Use the following commands to create a directory and move the database into it.
cd /tmp
mkdir uid ( Example : mkdir 94abc )
mv plate1.db /tmp/uid/. ( Example : mv plate1.db /tmp/94abc/. )
Then use the commands mentioned above. Once the database has been compacted quit from Patran and then move the database back to your home directory.
cd(this should take it to your home directory)
cd p3 (if you are working on a separate directory called p3).
mv/tmp/94abc/plate1.db .
________________________________________
Q2.6 : When I open existing PATRAN database the heartbeat continues to flash red indefinitely. What is the problem?
This can happen if using fvwm or one of its variants or Start or twm window manager in the HP teaching system. Find the process ID of the PATRAN process either using top or ps -eaf | grep "p3". Then killing the process off by typing kill -9 at a x-term window.
Exit from whatever window manager you were running and run the dtwm window manager and then open the PATRAN database in question. This should restore the database for use by the heartbeat turning to a steady green. However if this does not happen then the database is corrupt.
Then it might be possible to delete the database and then use the journal file (*.db.jou) to re-create the database. Under File... choose Utilities... and Rebuild and then choose the appropriate journal file.
________________________________________
Q2.7 : What do I need to specify to create a ABAQUS restart (*.res) file?
In the radio button Analysis form make the following selection :
Action : Analyze
Object : Entire Model
Method : Full Run
Click on Restart Parameters... . In the new form that pops up set
Restart Type : Write
Also set the parameter Increment between writing data to the appropriate number. Then click on the APPLY button.
________________________________________
Q2.8 : Why is that one has to give names to everything in PATRAN?
This is for easy grouping and assigning properties. If you have complex assembly with components having different physical and material properties then it makes it easier to assign different geometry groups when these components are created. Similarly the finite element entities when created could be in separate f.e. groups. This enables one to view and manipulate the groups individually and in combination.
The same applies when loading and boundary conditions are to be specified that these are also given meaningful names. Then these can be combined into one or more load cases.
________________________________________
Q2.9 : What is the significance of the names used for job, job step and load case in a ABAQUS analysis?
ABAQUS analysis consists of one or more STEPS. Each step consists of a load case. Whatever the loading and boundary conditions specified in a load case it is associated with a job step. A PATRAN job step corresponds to a ABAQUS STEP. The job steps have to be given names so that these can be selected. The names of the job steps also appears with each STEP in the ABAQUS input file.
If there are more than one step in the analysis then there should be one loadcase (and a job step) for each of the step. The loadcase name is used for identifying the results after the ABAQUS job has run and the results have been read into the PATRAN database ie during post processing.
The job name by default is the same as that of the PATRAN database. It is the name of the ABAQUS input file that will be created. For example if one is working on the database plate.db then the ABAQUS input file will be called plate.inp by default. However it need not be the same. For example if you are planning to run a number of analyses (say) for the purposes of a parametric study then the job name can be modified to represent this. Here "plate-a", "plate-b" are variants that can be used to represent different files but which is still associated with the riginal "plate" database.
________________________________________
3. Display
Q3.1 : How do I remove/add point/line/surface/node/element labels?
To remove all the labels from display use the "Hide Labels" icon .
Hide Labels icon
However if you want to selectively remove the labels (for example to remove only the node numbers) choose Display from the pull-down menu and then Entity Color / Label / Render.... In the form that pops up look under the heading "Entity Type colors and labels". Unset the entitites for which you want the labels to be removed and click on the Apply button.
To display all the labels click on the "Show Labels" icon in the toolbar.
Show Labels icon
To selectively display labels follow the instructions given above.
It is also possible to use the "Label Control Form" icon in the toolbar (this is a shortcut).
Label Control Form icon
Click on this and in the icon menu which pops up labels can be switched on and off selectively.
________________________________________
Q3.2 : How do I find the positive normal to a surface?
There are two ways to find the positive normal to a surface. The first method allows you to reverse the normal direction if required.
•        First method : Click on the Geometry radio button. Change the `Action' to `Edit'. The `Object' to `Surface' and the `Method' to `Reverse'. Click on the `Auto Execute' button to unset it to avoid any un-intentional reversal of normals. Click on the box marked `Surface List' and click on the surfaces for which you require the normals to be drawn. Then click on the box marked `Draw Normal Vectors'.
Use the middle mouse button to tilt the surface to see the normal clearly (hold down the middle mouse button and move the mouse). These vectors originate from the centre of the surface and are normal to the surface. Compare it with the positive direction of the appropriate axis (Z axis for plane problems).
If you need to reverse the normal direction click on `Apply'.
•        Second method : Choose `Display' from the top menu. Choose Geometry... and click on the label `Show Parametric Directions'. Then click on the `Apply' button. In one corner the parametric directions C1 and C2 (denoted by a set of axes and labels 1 and 2) will be displayed. Crossing C1 and C2 will give the C3 direction. Compare it with the positive direction of the appropriate axis.
________________________________________
Q3.3 : I have a 3D mesh displayed in wireframe mode. How do I get a hidden line or shaded view?
Short Cut : Click on the Hiden line icon from the Quick Pick icon menu to get the hidden line view. Click on the Shaded smooth icon from the Quick Pick icon menu to get the shaded view.

Alternatively choose Display from the pull-down menu and then Entity Color / Label / Render.... In the form that pops look at the box marked `Render Style'. Click on the current option (Wireframe) and choose from the menu options `Shaded/Smooth' and click on the `Apply' button to get a shaded plot.
Choose the option `Hidden Line' and then click on the `Apply' button to get a hidden line plot.
________________________________________
Q3.4 : I have zoomed in to part of the f.e.mesh and I am using the middle mouse button to rotate it and check it. But Patran automatically redraws the whole mesh to fit the viewport. How do I prevent this from happenning?
Choose Preferences from the pull-down menu and then choose Graphics.... In the form that pops up unset the radio button Auto Fit View and then click on the `Apply' button. This will prevent auto fitting when the view is rotated.
________________________________________
Q3.5 : How do I display the f.e.mesh with shrunken elements?
Choose Display from the pull-down menu and then choose Finite Elements.... In the form that pops look for a scroll bar marked FEM Shrink. The values are in fractions. Set it to the required value and then click on the button marked `Apply'. A value of 0.05 means 5 % reduction in size.
________________________________________
Q3.6 : I have a 3 dimensional model and I would like to spin it ie. rotate it slowly so that I can view it from different directions. How do I do that?
Choose Preferences from the pull-down menu and then choose Mouse.... In the form that pops click on the button marked Spin Model to set it. Now in the viewport hold down the middle mouse button anywhere in the viewport and move it in the direction in which you want to spin it and then release the mouse button. This should cause the model to spin. To stop the model from spinning click the middle mouse button.
The rate of spin is controlled by the amount of mouse movement when the middle button is held down. Move it by a very small amount before releasing it to spin the model very slowly.
The direction of spin is chosen by the direction of the mouse movement.
________________________________________
Q3.7 : When an entity selection has to be made the `Select menu' which usually appears next to the form does not appear ie pop up. What do I do ?
Choose Preferences from the pull-down menu and then choose Picking.... In the form that pops look for a button marked Popup Select menus and unset it and then click on Close. Then quit from Patran and then re-start it again for the change to take effect (it is not sufficient to close the database you were working on and then re-opening it).
The above change gets written to the settings.pcl file which is read when you re-start Patran.
________________________________________
Q3.8 : Can the default select entity cursor be changed to show a pair of crosswires?
Yes. Choose Preferences from the pull-down menu and then choose Picking.... In the form that pops look for the label Entity Picking Cursor. Click on the default cursor to reveal the choices. Make your choice and click on Close.
________________________________________
Q3.9 : Is it possible to change the centre of rotation?
Use the above icon to change the centre od rotation. Click on this first and then click on the point to be the new centre of rotation. If you are working with a 3-dimensional model then you may have to repeat this process a few times with change of viewing direction. This is because you cannot fix a point in 3-dimensional space with a single view. You need to "triangulate".
________________________________________
4. Display/Results
Q4.1 : When viewing the results how do I remove the undeformed mesh from view?
Click on Display Attributes icon (3rd icon) in the Results form. In the new form look for a button marked Show Undeformed and click on it to unset it. Then click on the Apply button.
________________________________________
Q4.2 : When viewing the results how do I remove the Patran default title which appears in the main viewport?
Choose Display from the top menu. Choose Results... and click on the label marked Show Result Title to unset it. Then click on the `Apply' button.
________________________________________
Q4.3 : How do I add my own titles?
Choose Display from the pull-down menu and then Titles.... In the form that pops look at the box marked `Target Title'. Enter the title you want to be displayed and click on the button marked `Create'. This should display the title on the viewport. Press the left mouse button on the new title you have added and move the mouse (while holding down the left mouse button) and this allows you to re-position the title. Any number of titles can be added by entering the title in the box and clicking on the `Create' button.
The re-positioning of the title is only possible when the Titles form is up.
The colour of the title and the size can also be changed. Click on the `Title Color' to change the colour and click on the `font size' to change the font size.
Titles can be deleted as follows. Click on the title to be deleted on the viewport using the left mouse button. This will display the title on the `Target Title' box. Click on the `Delete' button and click on `Yes' in the new confirmation window. This should delete that title from the viewport.
To change an existing title click on the title as before. Then click on the button marked `Rename'. In the new form type in the new title and then click on `Apply'.
________________________________________
Q4.4 : I have drawn the stress tensors first and then subsequently generated a fringe plot which appears superimposed on the previous plot. How do I clear the screen in between plots?
Before drawing the second fringe plot click on the `Reset graphics' icon in the top line (The 3rd icon - the "broomstick"). This should erase the previous plot.
________________________________________
Q4.5 : How do I get the fringe plot drawn on the undeformed mesh?
Click on the `Reset graphics' icon and this will clear and redraw the undeformed mesh. Any susbsequent fringe plot will be drawn on the undeformed mesh.
________________________________________
Q4.6 : How do I get the fringe plot drawn on the deformed mesh?
Click on the `Reset graphics' icon and this will clear and redraw the undeformed mesh.
In the Results form set `Object' to `Deformation'. Choose the Displacement results and then draw the deformed mesh. Now change the `Object' to \Fringe' and request the fringe plot and this will be drawn on the deformed mesh.
________________________________________
Q4.7 : How do I remove the element boundaries from the plot and just have the mesh outline?
Click on the Display Attributes icon (3rd icon in the Results form). In the form that is displayed look for the label Render Style. Change the entry for this from Wireframe to Free Edge and click on the Apply button.
________________________________________
Q4.8 : The deformed shape looks very distorted. How do I change the displacement magnification?
Probably the displacement magnification is too high. If you know approximately what the largest displacement is then you can use the direct multiplication option. If in create a fringe plot of the displacement to find the maximum. Alternatively you can set the largest displacement to be scaled to be 10 % of the largest dimension of the mesh.
Click on Display Attributes icon (3rd icon) in the Results form. In the new form look for Scale interpretation. Below this you will find 2 radio buttons marked Model Scale and True Scale. In the box below marked Scale factor enter a value of 0.1 which is the default. Click on the radio button marked Model Scale. Then click on the `Apply' button.
Also note that when you click on the `Fit View' icon it uses the undeformed mesh to fit the viewport ie it does not take into account the deformations. It does not use the deformed mesh to fit the view. Because of this in some cases part of the deformed will be outside of the viewport.
Fit View icon
________________________________________
Q4.9 : I am creating a fringe plot of the displacement magnitude. The plot looks OK but the legend displays zeroes for all the fringe bands. What do I do?
Most probably the displacements are too small to be displayed in the default fixed format.
Click on Display Attributes icon (3rd icon) in the Results form. In the new form click on Label Style.... In the form that pops up look for Label Format. It can have 3 choices : Exponential / Fixed / Integer. Chooese Exponential. Below that will be `Significant Figures' setting. Set the slider bar to the required value. Then click on `Apply'.
________________________________________
Q4.10 : In displaying the results some numbers appear superimposed. What are these and how do I remove them?
These could be the minimum and maximum values of the results parameter you are plotting.
This can be checked as follows :
Click on Display Attributes icon (3rd icon) in the Results form. In the new form look for the button marked Show Max/Min Values and if it is set then this would confirm it.
Click on it to unset it and then click on the `Apply' button.
________________________________________
Q4.11 : How do I change the number of fringe bands or the fringe interval?
Click on Display Attributes icon (3rd icon) in the Results form. In the new form click on Range.... In the new form click on Define Range....
Alternatively choose Display from the pull-down menu and then choose Ranges....
Both methods displays the same form. In the form that pops look at the boxes marked Data Method and Thresholding.
•        To only change the number of fringe bands
Click on the label Create... and in the form displayed below enter a title for New Range Name example : range10 (if you require 10 bands). Then change the Number of sub-range to 10. Then click on OK.
In the original form click on the label Assign Target Range to Viewport. Click on the labels Calculate and Apply respectively.
This should display the fringe plot with the required number of fringe bands.
•        To specify a start and end value.
This is shown in the following form. The number of intervals has been selected to be 10.

In the Data Method section Semi-Auto option is chosen. Click on Fit Results. This will display the maximum and minimum values in boxes marked Start and End. You can edit the start and End values to set these to the required range and then click on Calculate and then finally on Apply.
•        To specify a start and an interval value.
In the Data Method section choose Semi-Auto (Delta) option. Then enter the Start and the delta values and click on Calculate and then finally on Apply.
________________________________________
Q4.12 : Can the results values used in the fringe plots be scaled?
First create the fringe plot. Then in the Results form click on the 4th icon (Plot Options). In the new form change the Scale Factor from 1 to the required value. Then click on Apply. This should redraw the fringe plot appropriately scaled.
________________________________________
Q4.13 : How can I produce a contour plot (just lines) instead of a fringe plots (colour bands)?
Click on the radio button Insight and use the Contour Tool to create a contour plot. In the insight form choose the following options :
Action : Create
Tool   : Contour
Let us assume that we require a contour plot of von Mises stress. Click on the Results Selection... button and in the new form select Stress Components in the Results Selection box.
Then click on the button marked Result Options.... In the new form select the following option.
Tensor to Scalar Transform Method :von Mises
Click on OK on both these forms and then click on the Apply button in the insight form.
To change the contour interval click on the Insight Control pull-down menu and choose the option Range Control.... Minimum and maximum values can be set in the new form. Also the number of contour levels can also be set.
________________________________________
Q4.14 : I have carried out one analysis and looked at the results. I have modified the mesh and re-run the analysis and looked at the result and these are fine. However If I try to look at the results of the first analysis they look wrong. What do I do?
Once the finite element mesh has been changed it is not possible to go back and look at a previous set of results carried out with the different mesh.
Carry out all the post-processing with a particular mesh before making any changes to the mesh to run further analyses. Alternatively if possible it is better to use separate patran databases for different meshes and analyses.
________________________________________
Q4.15 : I have carried out one analysis with a coarse mesh. I would like to refine the mesh. On what basis do I refine the mesh?
The regions of the mesh which have high stress gradients should have finer mesh and are a good place to start with. Stress jumps take place across element boundaries. Stresses are accurately defined at integration points. The maximum difference in stress at any given node extrapolated from the elements shared by the node could be a good indication of the fineness of the current mesh. This is illustrated in the following figure :

This difference in stresses can be plotted as a fringe plot as follows :
In the Results form select the stress quantity for which you want to plot the maximum differences first (example : von Mises Stress). Then click on the 4th icon (Plot Options). In the new form, under the heading `Averaging Definition' change the Method to Difference.
Then click on Apply.
The regions where this maximum difference is high should be further refined.
________________________________________
Q4.16 : Is it possible to display the nodal values of the fring plot?
Yes it is possible. Create the fringe plot in the usual manner. Then
Choose "marker" for `Object' "tensor" for `Method'. In the Results form select the stress quantity for which you want to display the numerical values first (example : von Mises Stress). Then click on the Apply button.
This should display the numerical values at all the nodes.
________________________________________
Q4.17 : How do I get a shaded view of the deformed mesh?
In the results form select the displacement results first. Then click on Display Attributes icon (3rd icon) in the Results form. In the new form look for the option Render Style and set this to shade. Then click on the Apply button.
________________________________________

5. Geometry
Q5.1 : I have created a small arc (curve) and it is displayed by a `V' shaped line. What do I do?
Choose Display from the pull-down menu and then Geometry.... In the form that pops up look for a box marked Chordal Tolerance and the value of 0.005. This represents the maximum deviation (in the user used length units) from a curve. Change this to 0.0005 and then click on the Apply button. This should display the arc correctly.
Chordal Tolerance refers to the accuracy that will determine the number of straight line segments used when approximating curved lines.
________________________________________
Q5.2 : When I created a ruled surface with old versions of PATRAN green lines were drawn which represented the surface. Why are these lines absent with the latest version of PATRAN?
These green lines were a useful means of identifying the ruled surfaces. However these used to confuse some users finite elements.3 was the default no. of lines. Now the default is 0. You can change this number as follows :
Choose Display from the pull-down menu and then Geometry.... In the form that pops up look for a box marked Display Lines and the value will be 0. Change this to 3 and then click on the Apply button. Then click on the "Refresh" icon and this should display the green lines.
________________________________________
Q5.3 : How do I find the centre of gravity, volume, mass and 2nd moment of area of the geometry I have created?
Choose Tools from the pull-down menu and then Mass Properties.... In the form that pops up `Action' will be set to `show'. Set the `Dimension' to the appropriate setting. Choices are : 3D, 2D Axisymmetric, 2D Plane Stress, 2D Plane Strain.
Click on the button marked Define Region.... In the new form set `include' to Geometry. Change this to FEM if the objects are finite elements.
In the box marked Select Groups highlight the group or groups in which the objects reside. More than one group can be selected. Hold down the CTRL key and click on groups to de-select (if you have made a mistake).
Cick on OK in this form and in the original click on Write to report file if you want the requested information written to a file. This will bring up a new form for the report file name. You can choose the default file name (database-name.rpt.01) and click on the Apply button.
There are 2 boxes with the headings :
•        Density/Concentrated Mass
•        Thicknesses/Area
These can be set to either Use Element Properties (if element properties have been specified) OR Unity (if properties have not been set up).
Then click on Apply button in the original form.
________________________________________
Q5.4 : Is it possible to create a triangular surface?
Yes. In the `Geometry' form (radio button Geometry) choose the following :
Action : Create
Object : Surface
Method : Edge

option : 3 edge
Then click on the 3 edges which make up the triangular surface.
________________________________________
Q5.5 : I need to create a surface with curved sides. When I tried to create it using opposite sides it ignores the curved sides and creates a trapezium. How do I correct this?
If there are only 2 curved edges and if these form the opposite edges then choose the 2 curve method and then use the curved edges to create the surface.
For any other situation use the 4 curve method.
________________________________________
Q5.6 : I need to create a superimposed set of surfaces. How can I make a copy from an existing surface?
In the form Geometry make the following selections :
Action :Transform
Object :Surface
Method :Translate
Then use the translation vector < 0 0 0 >. Then click on Apply. When Patran puts up the warning message window click on Yes for All. It will be good idea to create a separate geometry group and have it posted before attempting to do this. If different material properties have to be specified to the newly created surface then this will be useful.
________________________________________
Q5.7 : In trying to create a graded mesh can I connect a corner point of one surface to the middle of another side?
The figure on the left shows a construction which is not permitted. Corner point of one surface connected to the middle of a side of another surface. The figure in the right shows the correct way of connecting the points and the surfaces.

Use the wireframe analogy in building up the mesh. Adjacent surfaces should share the side wholly not partly. Otherwise this will lead to mismatching nodes along these sides when the mesh is generated.
If the idea is to create a graded mesh and confine the density of elements to a local region then can use the following scheme to prevent propagation of geometry changes throughout the structure.

The above construction confines the density of the elements to the neighbourhood of surface 1.
________________________________________
Q5.8 : I am creating a new model and I am placing the different parts of the model in different groups. However the newly created surfaces, solids seems to end up in the wrong groups. What do I do?
Just before you create surfaces/solids which are to go into a separate group, create that new group. Look at the heading at the top of the viewport. This should have the (1) The Patran database name (2) Viewport name (usually default_viewport) (3) The current group names. The current group should be the newly created group. Then whatever entity you create (surface/soild) will be placed in that group ie the current group receives any newly created entities.
The problem arises when you want to add surfaces/solids to a previously created group. The correct procedure is to make that group current before creating the new entities.
Click on the top menu Group and select Set Current .... Then in the new form select the group (to which you want to add entities) from the list under the heading Set Current Group. Then click on Cancel.
The viewport heading should now display this group's name. Now post any other groups you need (example any groups which may contain the points/lines required) to create the surfaces/solids).
Click on the top menu Group and select Post .... Then in the new form select the required groups from the list under the heading Select Groups to Post. Then click on Apply. When you do this make sure that the heading does not change.
Finally the following procedure can be used to move the entities to the correct group. Click on the top menu Group and select Move/Copy .... Then in the new form select the group which has wrongly got the entities from the list marked From Group. Then select the group to which these should belong to from the list marked To Group. Then click on the radio button Move. Then click on Selected Entities.... In the new form click on the entity types you want to move under the heading Geom on. For example if you want to move only surfaces click on the square button marked Surfaces. This will display all the surfaces under the column marked Move. Edit this to list only the surfaces you want to move. Then click on OK. Then click on Cancel in the Group form.
Then post only this group and check the entities in that group.
Q5.9 : How do I create a circle (circular surface) ?
Create 2 points representing the centre of the circle (say Point 9) and a point on the circumference (say Point 11). Then in the Geometry form set : Create / Surface / Revolve.
Set the Axis to be through the center of the circle and perpendicular to the plane of the circle.
Axis : { Point 9 [ x9 y9 1] }
Here Point 9 is the centre of the circle. Point 9 and [ x9 y9 1] represents a line normal to the plane of the circle. Set Total Angle = 360. Click on the box marked 'Curve List' and then select the 2 Point icon from the select menu. Then click on Points 9 and 11 (which from the radius). The circle is denoted as surface 2 in the figure below.

________________________________________
Q5.10 : How do I create an ellipse (elliptical surface) ?
First create a circle as follows : Create 2 points representing the centre of the circle and a point on the circumference. Then in the Geometry form set : Create / Surface / Revolve. The follow the instructions given above and create the circle.
Change the setting to : Transform / Surface / Scale. Set the scale factors accordingly. For example to reduce the vertical axis (y) by half while keeping the horizontal axis (x) the same use : < 1.0 0.5 1.0>. Set the origin to the centre of the circle and then select the circle for the surface.
However if the axes of the ellipse are parallel to the original co-ordinate system then one needs to create a new co-ordinate system (Coord 1) with axes parallel to the axes of the ellipse. Choose : Create / Coord / Axis. Axis : Axis 1 and 2. Enter the co-ordinates for the origin and points on axis 1 and 2.
Origin : [ 0 0 0 ]
Point ox Axis 1 :[ 1 1 0 ]
Point ox Axis 2 :[ -1 1 0 ]
In the above example the new co-ordinate system is at an angle of 45 degrees to the original system. It will have the label Coord 1. Then transform the circle into an ellipse as before but use the new coord system.
Refer. Coordinate Sytsem : Coord 1
________________________________________
Q5.11 : How do I create a graded (unstructured) mesh with fine elements nearer the central hole in a thick cylinder problem ?
Here a segment created by two radial lines (and the inner and outer arcs) is used to illustrate the surface used. The outer radius is 30 and inner radius is 15. Along the radial lines 10 mesh seeds with One Way Bias towards the inner circle is assigned. Then along the outer circle 6 Uniform mesh seeds are assigned. Along the inner circle 10 Uniform mesh seeds are assigned. Then using the PAVER method Tri3 (3-noded triangle) elements were created.
Alternatively the above segment can be divided into a inner and outer surface using an intermediate circle (radius 15). For the outer surface mesh seeds are assigned in the same way as before.
For the inner surface the size of the elements can be controlled using Create / Mesh Control / Surface in the Finite Element form and assigning a Global edge length of 2.0. The created mesh is shown below :

________________________________________
Q5.12 : Can I use super-imposed surfaces for modelling a part of the mesh which is of different thickness?
Yes if the super-imposed surface maps onto a surface which exactly matches it then there shouldn't be any problem. This is shown in the figure below.

The surfaces shown on the right can be superimposed on the geometry shown on the left becuase there is an exact match. Whereas in the case of the geometries shown below the surfaces shown on the right cannot be super-imposed on the surfaces shown in the left. Because ther are no common points/lines/surfaces.

However there is no need to resort to the use of super-imposed surfaces just to specify a different thickness. PATRAN allows for different regions of the mesh to be assigned different thickness. It is sufficient to divide the region to be assigned a different thickness into separate surfaces. For example the inner annulus consists of 4 surfaces. These are separate from the rest of the geometry. The inner annulus (consisiting of 4 surfaces) can be assigned a different thickness from the one to the rest of the geometry. This eliminates the need for the use of super-imposed surfaces.
For 2D PLANE STRESS analysis this thickness is specified in the Properties form.
________________________________________
Q5.13 : I need to change some dimensions of the geometry and re-create a mesh. Are there any short-cuts?
There are couple of methods. First method is if the changes to be made are very few and suitable if intended to be carried out only once.
In this method one makes a copy of the original journal file under a different name. For example plate0.db.jou is copied to plate1.db.jou. Then edit this file and change the line which has the database name to correspond to the new journal file name. Then search for the dimensions you want to change and replace these with the new values. Then save and exit this file. The journal file is a text file and all these changes can be carried out using the standard text editor. It is also possible to edit and remove any sequence of commands that is not wanted. However be careful not to delete any lines which might be relevant any subsequent operation.
Then start up PATRAN in the usual manner and choose File / Utilities / Rebuild.... Then choose the newly modified journal file and click on Apply. This will run through the journal file and re-create the new mesh.
The second method is useful if you plan to carry out a series of parametric studies where a number of variables are to be changed and the planned changes are substantial.
Here the journal file from a original analysis is copied under a different name as before. Then all the values (whether it be dimensions or material properties or mesh division) which are to be changed are replaced with parametric names. Then these parameters are grouped together and set to new values towards the top of the journal file. This is illustrated with an example :
uil_file_rebuild.start("/export/msc/patran8/patran80/abaqus.db", @
"/amd_tmp/rasp-16/users3/abcd1/p8/pipe2.db")
db_set_pref( 303, 3, 0, FALSE, 0.00099999998, "" )
STRING asm_create_grid_xyz_created_ids
$ pipe outer radius
REAL pipe_out_rad
$ pipe inner radius
REAL pipe_in_rad
$ intermediate radius
REAL int_rad
$ final radius - marks the extent of the circular region
REAL fin_rad
$ no. of elements - layer (mesh divisions)
INTEGER lay_elno
$ no. of elements radiallyin a 45 deg segment
INTEGER rad_elno
...
$
pipe_out_rad = 0.5
pipe_in_rad = 0.487
int_rad = 0.7
fin_rad = 1.2
lay_elno = 3
rad_elno = 3
...
$#
asm_const_grid_xyz( "1", "", "Coord 0", asm_create_grid_xyz_created_ids )
$# 1 Point created: Point 1
asm_const_grid_xyz( "2", "[`pipe_out_rad` 0 0]", "Coord 0",@
asm_create_grid_xyz_created_ids )
$# 1 Point created: Point 2
asm_const_grid_xyz( "3", "[ `int_rad` 0 0]", "Coord 0",@
asm_create_grid_xyz_created_ids )
$# 1 Point created: Point 3
asm_const_grid_xyz( "4", "[ `fin_rad` 0 0]", "Coord 0",@
asm_create_grid_xyz_created_ids )
$# 1 Point created: Point 4
...
mesh_seed_create( "Surface 34.4 33.4 40.4 39.4 38.4 37.4 36.4 35.4 ", 1, `rad_el
no`,@
0., 0., 0. )
________________________________________
6. Finite Elements
Q6.1 : The f.e. mesh I have created has many more elements than I had expected. What do I do?
This usually happens due to sides which have not been assigned mesh seeds. On these sides Patran uses the Element length (L) to work out how many elements should be generated along the side. Click on the `Element Length' button and this will display the current setting.
Click on the button marked Display Existing Seeds to find out which sides have not been assigned seeds. Specify the mesh seeds along which many elements were generated. Then delete the current finite element mesh and re-generate it.
To delete the current mesh change the Action to Delete and then select the finite element mesh by drawing a box around the whole mesh.
________________________________________
Q6.2 : What do I do to get the current mesh seeds displayed?
In the Finite Elements form choose the following :
Action :Create
Object :Mesh seed
Type   :Uniform
Then click on the label Display Existing Seeds. This should display the current seeds. The number of yellow circles along each side represnts the no. of divisions.
________________________________________
Q6.3 : How do I go about assigning mesh seeds differently to different parts of the geometry? It seems tedious if the geometry is complex and has many surfaces?
You can hold down the Shift key when clicking on the sides. This allows you to make multiple selection.
Opposite sides of the surfaces are meshed identically. The following figures show the minimum number of sides for which the mesh seeds have to be specified.


Can you figure out why the 3 curved sides along the outer boundary (denoted by X) have not been assigned any mesh seeds?
________________________________________
Q6.4 : When making copies of surface already assigned mesh seeds does the information about the mesh seeds 'remembered' by the copies?
No.
________________________________________
Q6.5 : How do I add a concentrated mass?
Click on radio button Finite Elements and in the form make the following selection :
Action : Create
Object : Element
Method : Edit

Shape : Point
Then click on the node where you want to position the concentrated mass and then click on Apply. It should display a red triangle at this node.
Then click on the radio button Properties and in the form make the following selection :
Action : Create
Object : 0D
Method : Mass
In the box marked Property Set Name anter a name for the concentrated mass. Then click on the button marked Input Properties... and enter the mass of the element in the box marked Mass Magnitude and click on the OK button. In the original form click on the Select Members input field. Select the Point Element icon from the `Select Menu' and then click on the element created before (red triangle). Then click on Add and finally on Apply.
________________________________________
Q6.6 : I am trying to create a `Beam is Space' for use with ABAQUS and I am getting the following error message?
A Value for Property "Definition of XY Plane" must be entered. Check the remaining property values.
In the form that comes up when you click on Input Properties... in the Properties form you need to enter the gradient of the in the 1-direction in the box marked Definition of XY Plane. Enclose this in angled brackets. For example if the beam cross-section is rectangular as shown below :

Consider the 3 beams spreading out from a point radially (see plan view shown below). If each is of rectangular section then the gradient in 1-direction is as shown. This is the data that should be entered in the box marked Definition of XY Plane.

Even if the cross-section is circular you need to specify a direction for the above category.
________________________________________
Q6.7 : I am trying to create shell elements using the `Finite Element' form. The only choice I can make is the order of the element : Quad4, Quad8. What needs to be done?
At this stage just choose the appropriate order for the element. Example : Quad4 or Quad8.
Then in the form Properties choose the following options :
Action    : Create
Dimension : 2D
Type      : Shell
This will select the required shell elements. However if you require elements for Plane stress or Plane Strain then change the Type to 2D Solid.
________________________________________
Q6.8 : The geometry I have created is dividied into different groups. I want to create a new single group (say called `fem') to receive all the finite elements that will be generated. How do I do that?
Click on the pull-down menu Group and select the option Create.... In the form that pops in the box marked New Group Name enter an appropriate name (say fem and then click on the Apply button. Then click on the Cancel button to close that form. This will create the new group to receive the finite element mesh.
Click on the pull-down menu Group and this time select the option Post.... In the form that pops in the box marked Select Groups to Post click on the newly created group ( fem ) and click on the Apply button. You will notice the viewport cleared and the heading changing to the new group name.
Then holding down the Ctrl key select all the groups which contains the geometries (by clicking the left mouse button). Then click on Apply.
This should display all the geometries in the viewport. However the viewport heading should still be the name of the group created for the finite elements.
Now click on the radio button Finite Elements and assign mesh seeds to the side and create the mesh. Once the mesh has been created and click on the pull-down menu Group and select the option Post.... In the form that pops in the box marked Select Groups to Post click on the newly created group ( fem ) and click on the Apply button.
Now only the newly created finite element mesh should be on display (and none of the geometries).
________________________________________
Q6.9 : Is it possible to assign mesh seeds at points which do not follow the uniform / one way bias / two way bias options?
Yes there is a further option which allows one to assign mesh seeds at precisely the points at which these are needed. This is done using the Tabular option. Here the locations of the seeds are worked out in fractions w.r.t the length of the side and these are entered in a table.
________________________________________
Q6.10 : Can equivalencing be used to join the nodes from 2 different parts (of an assembly) created and imported from Pro/ENGINEER?
It is possible but not recommended. Because it is unlikely that the position of the nodes will coincide in the contact surface from the 2 sides. Equivalencing under these circumstances will only remove duplicate nodes which match from both sides. This will leave all other nodes which do not coincide. This will be unsatisafctory if the coincident nodes are very few.
If using ABAQUS it is preferrable to define a contact pair and then use the option TIE then it will have the same effect as applying equivalence if all the nodes in the contact surface were coincident.
________________________________________
Q6.11 : Is it possible to create an unstructured 2-dimensional mesh?
Yes it is possible to create an unstructured mesh using the paver option. In the Finite Elements form choose : Action / Option / Type = Create / Mesh / Surface. Then choose the radio button Paver instead of Isomesh.
Similarly for 3-dimensional mesh choose Tetmesh instead of Isomesh.
________________________________________
Q6.12 : Is it possible to create an unstructured mesh made up of quadrilateral elements?
Yes it is possible to create an unstructured mesh consisting of quadrilateral elements.
See the answer to the question Q6.11.
________________________________________
Q6.13 : I have imported a cylinder (as part of an assembly) from Pro/ENGINEER but I cannot mesh it using brick elements. Why is that?
Yes. It is not possible to mesh a cylinder into brick elements if the cylinder was created in Pro/ENGINEER. The reason is that any object created in Pro/ENGINEER whether it be a cylinder or rectangular solid are "General Trimmed Surfaces" and these are coloured Magenta. These solids can only be meshed with the option 'tetmesh' ie tetrahedras.
________________________________________
7. Loads/Boundary Conditions
Q7.1 : How do I display the icons (markers) denoting loads and displacement fixities for checking?
Choose Display from the pull-down menu and then Load / BC / Elem Props.... In the form that pops up look for a button marked Show on FEM only and click on it to set it. Also click on Show All. Then click on the Apply and Cancel buttons respectively.
Click on the radio button Loads/BCs and change the `Action' to Plot Markers. Under the heading marked Assigned Load/BC Sets select the boundary conditions and loadings you want to be displayed. In the Select Groups category select the groups which has the finite element entities. Then click on the Apply button.
________________________________________
Q7.2 : How do I remove the icons (markers) denoting loads and displacement fixities from display?
Choose Display from the pull-down menu and then Load / BC / Elem Props.... In the form that pops up look for a button marked Show on FEM only and click on it to unset it. Then click on the button marked Hide All. Finally click on the Apply and Cancel buttons respectively.
This should erase the markers. If not click on the Reset graphics icon in the top right hand corner. It is the 3rd icon.
________________________________________
Q7.3 : How do I fix a node in the y direction only i.e. it is free to move in the x direction?
Enter < , 0 > in the box marked Translations .
The first , (comma) indicates that the degree of freedom in direction 1 is free. If this was a 3-dimensional example then the 3rd degree of freedom is also free becuase it has not been specified. In the above example the 2nd degree of freedom is fixed at 0.
________________________________________
Q7.4 : I have created a series of surfaces and then trying to apply uniform pressure (u.d.l.) to one side of these surfaces but in some surfaces it is directed in the wrong direction?
Check the Normal directions to these surfaces using the answer to Q3.2 above.
The applied positive pressures are directed in the direction of the positive normal. Applying a negative pressure will be in the direction opposite to it.
________________________________________
Q7.5 : I want to apply self-weight of the elements as loading. How do I do that?
Create a set of material properties in the usual manner. Make sure you specify the density.
Click on the radio button Loads/BCs and and in the form make the following selection :
Action :Create
Object :Inertial Load
Type   :Element Uniform

New Set Name : Enter a appropriate name - example : self-wt

Target Element Type :2D or3D (Make the appropriate choice)
Click on the button Input Data... and in the new form in the box marked Trans accel enter < , -1. , > asssuming the gravity is acting in the negative Y direction. Click on OK in that form.
In the orinial form click on the button Select Application Region... and in the new form select the radio button Geometry or FEM for the `Geometry filter'. Then select the elements or surfaces/bodies. Click on Add and then finally on the OK button.
In the original form click on Apply. This should display yellow arrows pointing in the direction in which the gravity is acting and the magnitude (for this example it will be 1).
________________________________________
Q7.6 : How do I apply a line load?
It is not possible to apply line loads along curves/lines directly.
The user may have to calcualte the equivalent set of point loads for the individual nodes and specify these as point loads.
If the element sides are 2 noded then the line load is split equally between the 2 nodes. If there are a series of sides then mutiply the line load by the length of the side and apply half to each node. Interior nodes will take contribution from the sides at either side.
If the elements are 3 noded then the total load (line load multiplied by length) is split in the ratio of 1 : 4 : 1 between the nodes. The centre node taking 2/3 rd of the total load and the end nodes 1/6 th of the total load. Again sum the contribution from either sides for end nodes in the interior.
For higher order elements similar factors can be calculated using the shape functions and the principle of virtual work (see any standard book on finite elements).

________________________________________
Q7.7 : Is it acceptable to assign boundary conditions on curves/lines not used in specifying the geometry?
No. If you are assigning boundary conditions on the geometry then you have to assign it on curves/lines used in specifying the geometry.
Consider the situation where lines L1 ans l2 form part of the surfaces which define the geometry (in the figure below). Assume that you also have defined a line L3 which connects points 1 and 3.

Consider the situation where the vertical side between points 1 and 3 is to be retstrained from moving in the horizontal direction. Then this boundary condition should be specified on lines L1 and L2 but not L3 (as a short cut). the reason is when the finite element mesh is created lines L1 ansd l2 are associated with the nodes that are created. Line L3 is not associated with these nodes.
If you attempt to specify the boundary condition on L3 only the nodes at points 1 and 2 will be asssigned that boundary conditions. All the intermediate nodes between points 1 and 3 will not be assigned the boundary condition.
________________________________________
Q7.8 : How can I specify the Load Proportionality Factor for a RIKS analysis step?
In the Analysis form make the following selections :
Action :Analyze
Object :Entire Model
Method :Full Run
Click on Step Creation.... In the new form set
Solution Type : Nonlinear Static
Then click on Solution Parameters.... In the new form set
Riks Method = ON
Stopping conditions : max Load Multiplier
Max Load Multiplier : 1.0
________________________________________
Q7.9 : How can I specify a triangular pressure distribution?
You need to create relationship (variation) using the FIELD form.
This is illustrated with an example :

First of all choose the following settings :
    Action / Object / Method:Create/Spatial/ PCL Function

    Field Name : < Enter an appropriate name here> Example : pressure

    Field Type :<> Scalar<> Vector
Choose Vector for prescribed displacement specification. Choose Scalar for pressure variation.
    Co-ordinate System Type :<> Real<> Parametric
Choose REAL if using the co-ordinates of the new system.
Here the default co-ordinate system (Co-ord 0) which is halfway up the side is not suitable for specifying the pressure variation. It is simpler to create a co-ordinate system with origin coinciding with the base of the side. Lets call this Co-ord 1.
Co-ordinate System : Change the default (co-ord 0) to co-ord 1.
Since the pressure variation is scalar enter the relationship in the box marked "Scalar Function".
    Example :p =( 10. - 'Y ) * ( 150. / 10. )

               =( 10. - 'Y ) * 15.
Here click on the appropriate independent variable ('Y) from the box of the same name whenever you want to use one of this variable in the equation.
Now click on APPLY to complete creation of the field.
Then open the LOADs/BCs form and give the pressure distribution a name and choose 3D for "Element Type". Then click on the Input Data.... In the new form the name of the previously specified pressure relationship (press) will be listed under the heading Field.
Click on the box marked "Uniform Pressure" and then click on "pressure" entry from the "field" section. Then click on OK and complete the form in the usual manner.
________________________________________
Q7.10 : How does one deal with the interface conditions between parts (of an assembly) imported from Pro/ENGINEER?
One can use contact pair option to identify the two surfaces in contact and then specify the interfcae conditions (smooth, frictional or bonded/tied).
Use the Loads/BCs form and choose : Action / Object / Type = Create / Contact / Element Uniform. Then choose Deform-Deform for "option" for contact between two deformable bodies.
Enter a meaningful name for the contact pair you are about to define, in the box marked New set name.
Click on Input Data... and in the new form choose the contact type to be either General or Tied. Enter appropriate values of Frictional coefficient and limiting shear stress if General was chosen. Initial adjustment tolerance also needs to be specified for both types of contact. Choose a value of about 1% of the largest dimension for this. This is the amount the position of the nodes on either sides can be adjusted to establish contact. Click on OK on this form and then in the main form click on Select Application REgions....
In the new form leave both master and slave surfaces at solid Face if dealing with 3-dimensional solids. If shell elements are involved then it can be set to shell surface.
Set active region to master and then choose the contact surface on the master component. If components of different materials are coming into contact then in general the stiffer of the two is selected as the master.
Similarly set active region to slave and then choose the surface which comes into contact on the slave component. Note that "master" can penetrate into "slave". Also the slave surface should have a more finer mesh. Once both sets of surfaces have been identified click on OK and then in the main form click on Apply.
In a complex assembly with several components there will be several sets of contact pairs needs defining. Repeat this procedure for each pair of such contacts.
________________________________________
Q7.11 : Given the choice of specifying the boundary conditions either on the geometry or on the finite elements which is preferrable?
In general it is preferrable to specify the boundary conditions on the geometry. This way if you decide to chnage the mesh at a later stage then the boundary conditions need not be re-specified.
However there are situations where there is no choice but to deal with the f.e.mesh. For example consider the situation where a point load is to be applied to node which is coincident with a point which has been used in the generation of the geometry. Then you need to create the mesh and then apply the load to the node in question. Alternatively create the geometry which will give a coincident point where the concentrated load is to be applied apply it the point
Here is a different example : Equal bending moment has to be applied to all the nodes on a particular face. Here the total bending moment is to be equally divided amongst all the nodes. Here one needs to work out how many nodes there is ging to be. Then apply the bending moment divided by the number of the nodes to the geometry.
________________________________________
Q7.12 : I need to apply a radial pressure to a circular hole in a plate for an imported mesh. Is there a simple way of selecting all the nodes along the circular hole?
Click on Tools and then choose List / Create. In the Create List Form set Model / Object / Method = FEM / Node / Attribute. Then choose the Coord value for Attribute. The box marked Refer. Coordinate Frame will have Coord 0 by default. If the default coordinate system's origin is at the center of the circular whole then the default is OK. If not create a coordinate system (called Coord 1) at the centre of the circular hole using the Geometry form and the settings : Action / Object / Method = Create / Coord / Axis. Choose a cylindrical co-ordinate system.
In the list form chnage the cordinate system to : Coord 1. Select x and this will display a new box for x value. In cylindrical co-ordinate system x would represent the (first) radial co-odrinate. So set the X value to be the same as the radius of the circular hole. Also set the TOL-XYZ to an appropriate value so that only the nodes along the circular hole will be selected. Check that the radio button for Target List is set to A. Now click on Apply. Now click on Add to Group... in the 'List A' form. The 'lista' contents should hopefully have all the nodes along the circular hole. These nodes can be highlighted and cut and pasted into any Select Application Region for nodes for applying a radial load in the Loads/BCs form.
________________________________________
8. Materials
Q8.1 : Is there are library of properties for standard materials?
No.
________________________________________
Q8.2 : I have an object which consists of 2 different materials. How do I specify the different materials?
Create 2 separate Geometry groups and construct the geometry separately. Using the Materials form define the 2 materials. Then post one geometry group only and using the Properties form select the appropriate material from the form which comes up when you click on Input Properties.... Both materials will be listed in th box marked Material Property Sets.
When assigning this set of properties to the geometry select the `geometry' icon from the `select menu'.
Now post the other geometric group and repeat the above steps.
________________________________________
Q8.3 : I am doing a plane stress analysis and the geometry even though consisting of a single material has 2 regions with different thicknesses. How do I specify these?
Define the material properties in the usual manner using the Materials form.
Create 2 separate Geometry groups and build the geometry with different thicknesses separately.
Click on the radio button Properties. Give the property set a name and then click on the Input Properties... button. Select the previously defined material from the Material Property Sets and enter the appropriate thickness in the box marked Thickness. Click on OK.
In the original form in assigning this set of properties to the geometry select the `geometry' icon from the `select menu'.
Now post the other geometric group and repeat the above steps.
________________________________________
Q8.4 : What constitutive models are available?
Click on the radio button Materials and click on the option Isotropic Object. This will reveal the following options :
Isotropic
2d Orthotropic (Lamina)
3d Orthotropic
3d Anisotropic
Composite
Click on the button marked Input Properties.... Then click on Elastic for the Constitutive Model category. This reveals the following choices if Elastic was chosen.
Elastic
Hyperelastic
Viscoelastic
Deformation Plasticity
Plastic
Failure
Creep
Thermal
If a selection other than Elastic is made on the original form then an appropriate subset of the above constitutive models will be available for selection.
________________________________________
Q8.5 : How can I check what different materials have been assigned to the finite element mesh?
In the form Properties make the following selections :
Action :Show

Existing Properties : Material Name

Display Method : Marker Plot

Select Group : Select the finite element mesh group
Then click on Apply.
________________________________________
Q8.6 : How can I check the material properties already defined?
In the form Materials make the following selections :
Action :Show

Existing Materails : Make a selection from the list
Click on Show Properties...
This will display the properties already defined.
________________________________________
9. Properties
Q9.1 : How can I check what properties have been assigned to which elements?
In the form Properties make the following selections :
Action :Show

Existing Properties : Material Name

Display Method : Marker Plot

Select Group : Select the finite element mesh group
Then click on Apply.
This would display a plot showing which elements have been assigned what.
Repeat this process by selcting another item under the heading "Existing Properties".
________________________________________
11. Analysis
Q11.1 : How do I carry out a dynamic analysis?
There are a number of different dynamic analyses that can be carried out. See the answer to Q1.3 on the available analysis types.
________________________________________
Q11.2 : How do I carry out a frequency analysis?
Click on the radio button Analysis and in the form that comes up click on Step Creation.... Click on the button marked Linear Static for Solution Type and select Natural Frequency.
Click on Solution Parameters. It will bring up the form listed below. Enter the required Number of Modes and then click on OK.

________________________________________
Q11.3 : How do I carry out a buckling analysis?
If using ABAQUS you need to create 2 steps. Step 1 is used to specify and Dead Load that is present. Step 2 is used to specify the Live load which is usually a unit load. For the second step follow the instructions given below.
Click on the radio button Analysis and in the form that comes up click on Step Creation.... Click on the button marked Linear Static for Solution Type and select Bifurcation Buckling.
Click on Solution Parameters. It will bring up the form listed below. Enter the required Number of Eigenvalues and then click on OK.

________________________________________
Q11.4 : How do I specify a non-linear analysis step?
In the Analysis form make the following selections :
Action :Analyze
Object :Entire Model
Method :Full Run
Click on Step Creation.... In the new form set
Solution Type : Nonlinear Static
Then click on OK in that form.
________________________________________
Q11.5 : How do I turn off the Perturbation option in a STATIC step?
In the Analysis form make the following selections :
Action :Analyze
Object :Entire Model
Method :Full Run
Click on Step Creation.... In the new form set
Solution Type : Linear Static
Then click on Solution Parameters.... In the new form set
Linear Perturbation Analysis : OFF
Then click on OK in that form.
________________________________________
Q11.6 : In trying to open the analysis form getting the following warning message : The PCL library file, mscnastran.plb, which would typically be associated with the current analysis preference, MSC/NASTRAN, does not exist?
This can happen if you forgot to change the template when creating a New database. Then by default MSC/NASTRAN becomes the default analysis module. However at CUED MSC/NASTRAN is not licenced, hence the above error message.
When creating a new database always change the template to whichever analysis module you are using (ABAQUS or MSC/PATRAN_FEA). For a previously created database you can also choose Preferences / Analysis... and then set Analysis Code to the appropriate code.
________________________________________
12. Results
Q12.1 : I have carried out an analysis of a static loading on a curved surface and the obtained displacements are small compared to the magnitude of the loading. What could be wrong?
For 3-dimensional curved surfaces the appropriate choice of element type is shell elements and not Plane Stress elements in the Properties form.
If this is a ABAQUS analysis look at the abaqus input file (*.inp) using a separate window and look for the presence of *SOLID SECTION. If found this would confirm the mistake. The number in the next line is the thickness of the element.
If making the changes directly on the abaqus input file replace the keyword using *SHELL SECTION and in the next line after the thickness add the number 5 (which represents the default number of section points).
For example replace the following
*SOLID SECTION
   10.
with
*SHELL SECTION
   10.,   5
However if you do this the patran database will be unaware of these changes. Alternatively these changes can be made in the database. This is the recommended way.
Click on the radio button Properties and select the following options :
Action : Modify
Object : 2D
Method : 2D Solid
Then change the 2D Solid to Shell and select the previously defined property sets and then click on Apply. This should change the element types to Shell elements.
________________________________________
Q12.2 : Can the results values be scaled?
If the results are curves created using XY Plot option then these can be scaled. However if these are values used in fringe plots then see the answer to question Q4.12.
________________________________________
Q12.3 : How can I delete the results from the Patran database after post processing?
In the Results form select "Action" to be Delete. Then Then set "Object" to Result Cases. In the box marked "Existing Result Cases" select the results you want to delete. Then click on Apply.
________________________________________
Q12.4 : I have used the Shell elements (S4R5) with 5 section points in an ABAQUS analysis. How do I generate a fringe plot of the stress results at section point 5?
In the Results form look for "Position". This will be set to At Section_Point_1. Click on this and a new form which will list all the section points for which the results are available.
Select the `Section Point 5' and click on the `Close' button. Then click on Apply.
________________________________________
Q12.5 : If I want to carry out a simple calculation ie calculate the mean of sig-xx and sig-yy stresses and produce a fringe plot of the results how do I do that?
In order to use the following procedure you need to have the shareware library loaded first. See the answer to question Q17.1 on how to do this.
From the top menu click on Utilities. From the menu that pops up select Results and Results Toolbox... respectively.
In the new form select Element and Scalar under Result Entities. This is because we are dealing with stress components. The intention is to calculate the mean of sig-xx and sig-yy. This is carried out in two stages. Stage one is to sum the 2 stress components. Part 2 is to multiply the results by a factor of 0.5.
The idea is to load the sig-xx values into register Res1 and sig-yy into Res2. In the box marked Element List enter the range of the elements to be considered in the calculations.
For Derivation click on the current option and choose XX. For Location choose As is. Click on Load Result.... In the new form select the load case from the list of loadcases. In the box marked subcases select the appropriate case.
Enter meaningful labels in the box marked Primary Result Label and Secondary Result Label. This will be used in identifying the new results. Finally click on OK.
Set the Calculated Results into Register to be Res3. Register assignment Method should be set to the = (equal) sign.
Register : Res1operator : +Register : Res2
Click on Calculate and the results will be written to register Res3. The next step is to multiply the results in register Res3 by 0.5 and place the results in register Res4.
Change the Calculated Results into Register to be Res4.
Register : Constantoperator : *Register : Res3
In the box below Constant enter a value of 0.5. Click on Calculate. The results will be in register Res4.
Ensure For Results in Register is set to Res4. Click on Save... and the newly calculated results will be saved.
________________________________________
Q12.6 : I am trying to create a graph plot along a surve and and getting the error message : "No F E Entity could be found in results post processing". What is the problem?
Make sure the finite element mesh is posted. You can get this message if you have posted ony the geometry group.
________________________________________
Q12.7 : I have read the results from ABAQUS back into the PATRAN database but when the results case was selected there was nothing in the box marked "Select Deformation Result" (for Object : Deformation). What is the problem?
It is very likely that that ABAQUS *.fil must be incomplete (for example due to exceeding your disk quota). This can be checked very easily by looking at the *.log file to see whether there were any problems with the analysis.
________________________________________
Q12.8 : I am trying to read the results from ABAQUS back into the PATRAN database but the heartbeat continues to flash red indefinitely. What is the problem?
See answer to question
Q2.6.
________________________________________
Q12.9 : In modifying an existing finite element mesh what shall I do with the old results?
Delete the results, otherwise this will lead to confusion later.
________________________________________
Q12.10 : The deformed shape looks strange. What could be the problem?
Three possibilities : If the mesh appears to be "breaking up", "flying apart" (ie falling to bits) then probably you have forgotten to "equivalence".
The second possibility is that the wrong results s being post-processed with the wrong mesh. This can happen if you have run an analysis and then modified the mesh and run a new analysis and then by mistake tried to plot the deformed mesh of the original results. It is always a good idea to delete all old results if you going to modify the mesh and run a new analysis. The results get accumulated in PATRAN and do not get automatically deleted when the mesh is deleted.
The third possibility is that the displacement magnification is too big. Reset the magnification to 1 and then try re-drawing the deformed mesh.
________________________________________
Q12.11 : I have carried out an ABAQUS analysis using 8 noded brick elements (C3D8) to find the eigen modes and eigen values. These results do not agree with experimental results. Why is that?
The lower order element is not suitable for bending problem. This could be due to shear locking. If using the lower order element in bending problems use the incompatible mode elements. In the properties form set : Action / Object / Type = Create / 3D / Solid. Change the Standard Formulation to Incompatible Modes.
Alternatively use higher order elements (C3D20).
________________________________________
14. XY Plots
Q14.1 : How do I get the results/data from a XY Plot into a file?
It is assumed that you have created a XY Plot and this is displayed on XYWindow1. It is also assumed that you have given a unique title to the curve or curves.
Click on the radio button XY Plot and in the form that pops up make the following selections.
Action :Modify
Object :Curve
In the box marked Curve List click on curve(s) you want to extract the data from (It should then be shown highlighted). Click on the label marked Data from keyboard....
In the new form click on the button marked Write to data file to set it and then click on Apply. This should bring up the Write Curve Data File form. Enter a name in the box marked Write XY Data to File and give it the extension xyd (example : disp.xyd) and then click on the OK button. If necessary you can include a title by typing it in the box marked XY Data Title.
This will create a file of the said name in the directory from which Patran was started. The first line of this file will have the label XYDATA and this will be followed by the title you had typed in. This is followed by the x and y values in the subsequent lines.
________________________________________
Q14.2 : How do I read in my experimental results into patran so that a plot comparing f.e. results with experimental results can be generated within Patran?
The data you want to read should be given a file name extension xyd. The first line should have XYDATA, this should be followed by a unique title. The rest of the data should be in pairs of x and y values separated by at least a space and one set per line.
This forms one set of data. Another set can be included starting a line with XYDATA, and another title. This is followed by the data. Any number of similar sets of data can be included following this format in the same file.
Click on the radio button XY Plot and in the form that pops up make the following selections.
Action :Modify
Object :Curve
In this form click on the button marked Data from File and then click on Apply. This should bring up the Curve Data File form.
The file which contains the data (if it had been given the extension name xyd will appear in the box marked Data files. Select it by clicking on it. Its name should appear in the box marked Read File. If your data file has only 1 set of data then click on the label marked Read. If there is more than one set of data then you can choose the appropriate set by entering its number in the box marked Set Number before clicking on Read.
This will display the plot in XYWindow1. It appears that the read curve is always displayed in XYWindow1. Therefore it will be a good idea to read in the curved data from another source (experimental, analytical) first and then create the XYPlots in Patran in XYWindow2. Then to make comparison post both the XYWindows.
It appears that read curves are not displayed under the list of curves. The reason for this is being investigated.
________________________________________
Q14.3 : How do I get a hard copy of an XYPlot?
Click on the pull-down menu File and select the option Print.... In the form that pops up change the the category from Current Viewport to Current XY Window. Check that the `Available printers' is DPO Postscript Printer. Even though you may not be sending the plot directly to the printer if you need postscript or encapsulated postscript output you need to choose this option.
Click on the label Options... and in the new form click on the radio button to make your choice. Click on Print to file for postscript and click on Create EPS File if you require an encapsulated postscript file. Leave both options unset to send the output directly to the printer. Click on the OK button.
In the original print form click on the Apply button. This will create an output file or directly send it to the plotter depending on your choice.
________________________________________
Q14.4 : I have created many XYWindows and when trying to tidy by deleting some of the XYWindows using the xterm delete option caused Patran to crash. What should I do?
It is not a good idea to get rid of the XYWindows using the xterm window `delete' option. One approach is to shut these down by unposting these windows.
Click on the radio button XY Plot and in the form that pops up make the following selections.
Action :Post
Object :XYWindow
If you want to remove all the XYWindows from view then click on the first XYWindow in the box marked Post/Unpost XYWindows. This will be the only one shown highlighted. Then holding down the Ctrl key click on the highlighted XYWindow to deselect it. Now none are selected.
Then click on Apply and this should remove all the XYWindows from view (but not delete it).
To re-display these XYWindows, highlight these and then click on the Apply button.
________________________________________
Q14.5 : I tried to create a new XY Plot and all 3 XYWindows had the newly created plot. The old plots in XYWindows 1 and 2 were overwritten by the new one. What do I do?
This happens because all 3 XYWindows are posted when you created a new plot. Before creating a new plot in a new XYWindow you should Unpost all the `existing' XYWindows.
Click on the radio button XY Plot and in the form that pops up make the following selections.
Action :Create
Object :XYWindow
In the box marked Enter XYWindow Name type in the new XYWindow you intend to create. Keep the numbers in sequence. Don't be tempted to skip numbers in creating new XYWindows. XYWindow4 should follow XYWindow3 and so on. Click on Apply.
Then change the `Action' to Post. Click on the newly created XYWindow in the box marked Post/Unpost XYWindows. This will be the only one shown highlighted. Then click on Apply and this should remove all the XYWindows except for the newly created one from view.
Now use the XY Plot in the Results form and create the new plot and give the newly created XYWindow name to it. Then the plots previously created in the XYWindows should not be overwritten.
________________________________________
Q14.6 : How do I add titles to the axes in a XY Plot?
Click on the radio button XY Plot and in the form that pops up make the following selections.
Action :Modify
Object :Axis
Click on X under Active Axis. Click on the label marked Title.... In the new form Click on the square button maked Display Axis Title. Type the X-axis title in the box marked Axis Title. You can change the character size by changing the Font Size. Click on Apply and then on Cancel.
In the original form now click on Y under Active Axis and then repeat the steps to add a title to the y axis.
Options... can be used to change the line style and line thickness of the axis. Scale... can be used to choose a linear or logarithmic scale. Labels... can be used to change the number of digits used in the display. Tick marks... can be used to change the no. of major and minor tick marks displayed. Grid Lines... can be used to display grid lines.
________________________________________
Q14.7 : In creating a new XYWindow Patran crashed with the following message - Error : Object " " does not have a windowed ancestor?
In creating new XYWindows give it a number in the ascending order without skipping any of the numbers in the sequence. XYWindow2 should be created after XYWindow1. Similarly XYWindow3 after XYWindow2.
Missing this sequence or even un-posting all previously created XYWindows when a new XYWindow is created can also cause this error. Also do not delete XYWindows1 and 2 before creating XYWindows3. This may also trigger a Patran crash with the above error.
Restart Patran and continue the session.
________________________________________
15. Hardcopy
Q15.1 : How do I get a colour postscript paper copy of size A1/A2/A3/A4?
Click on the pull-down menu File and select the option Print.... In the form that pops up make sure that DPO Postscript Printer is highlighted in the `Available Printers' box. This allows for a postscript plot to be created.
Click on the label Page Setup... and in the new form select the appropriate Paper Size. Then click on OK.
In the original print form click on the label Options.... In the new form change the format to Color. Then click on the Print to file option to write to a file. If choosing colour output it has to be saved in a file. It cannot be sent directly to the plotter. Click on the OK button. In the original form click on Apply.
This will create a postscript file. The name of the file will be listed in the history window. In a separate XTERM use the ghostview command to check the created plot file. If the size is greater than A4 you may only see part of the plot. If the plot appears OK then you have 2 choices.
(1) If the plots are A4 size then you can use the A4 colour laserjet printer using the following command :
lp -dcljmr1 file-name
(2) For all other sizes use the following command to sent the plot to the Designjet 1055CM plotter.
lp -dpltmr2 -oan file-name
Here replace the n with the paper size. For example if sending an A3 plot type :
lp -dpltmr2 -oa3 file-name
Please note that there is charge made for the use of the HP Designjet 1055CM plotter.
________________________________________
Q15.2 : How can I create a paper copy of a plot of size 200 mm x 100 mm?
Follow the instructions given above. In the form that pops up when you click on Page Setup... set the Format to Custom.
Change the Default Units to cm. Then in the box marked Width enter a value of 20 and in the box marked Height enter a value of 10. Then click on the OK button.
In the original print from click on Apply.
________________________________________
Q15.3 : How do I send the plot to an alternate destination?
Click on the pull-down menu File and select the option Print.... In the form that pops up look at the `Available Printers' box to see whether the alternate destination is listed there. If it does select it. If the printer to which you want to send the plot is not listed and after making sure that the said printer is connected to the same network and can handle postscript files, enter the printer name in the box marked Destination.
Click on the label Options.... In the new form ensure that none of the two radio buttons marked Print to File and Create EPS File are selected. Then click on the OK button.
In the original print form click on Apply.
________________________________________
16. Help
Q16.1 : How do I access the on-line help information?
Choose the pull-down menu Help and select the Document Library .... All the on-line documentation is accessible from the page which pops up.
________________________________________
Q16.2 : How do I get context sensitive help?
Place the cursor on the form for which you want help and press the F1 button. This should bring up the relevant help page. When finished click on the done button. However it is a good idea to leave this open because for subsequent requests the response will be much quicker.
________________________________________
Q16.3 : How do I access the on-line Examples?
Choose the pull-down menu Help and select the Document Library .... Choose Part 10 : Example Problems. The following 3 examples are available :
•        Fiber Optic Cable
•        L-Shaped Bracket
•        Spool
________________________________________
Q16.4 : How do I get hard copies of the on-line documentation?
When the relevant help page you want to print is up click the right mouse button and from the menu which pops up choose the Print... option.
In the new form click on the radio button All if you require all the pages in the section you are currently looking at. If you require only a few pages then click on radio button Start Page. Enter the starting and finishing page numbers in the appropriate boxes. You do not have to enter the section numbers preceding the page numbers. For example if you require pages 6.1 to 6.7 simply enter 1 and 7 respectively. This is assuming that you were looking at section 6 in help when you invoked the `Viewer' command. If you make any mistakes use the `Back space' key.
Click on the button next to `Last sheet first' to unset it. Click on the button next to `Print only to file' to set it. In the box next to it the default file name will be displayed. Place the cursor at the first character and double click the left mouse button. This should highlight the file name. Press the `back space' key to delete that. Enter a file name `section6.ps' in that box.
Check the printer paper size. The width should be 8.268 inches and the height 11.693 inches. If these are not then change them to these values. Reduce the scale to 80%. Make sure that the number of copies is 1. Then click on the OK button. This would create the postscript file. Use ghostview to check the postscript file before sending it to the laser printer. Use this facility sparingly and only print the essential information.
lp -dljmr1 -opostscript section6.ps
To delete the created file (after printing) type : rm section6.ps.
________________________________________
17. Miscellaneous
Q17.1 : How do I access the shareware available in Patran?
You need to set up a link as follows in order to use the shareware. In your HOME directory type :
ln -s /export2/patran3/shareware/msc/unsupported/utilities/p3epilog.pcl p3epilog.pcl
This will load the shareware library everytime you start up Patran. This link can be removed as follows :
rm p3epilog.pcl
When you start up Patran a new menu called Utilities should appear as part of the top menu. In using the shareware please note that there is on line help available.
________________________________________
Q17.2 : How do I access the spreadsheet program available in Patran as shareware?
See answer to the question Q17.1 on how to load the shareware first.
Then once Patran is up you will see Utilities menu on the top line. Click on it. From the menu select General and then Spreadsheet.... This will bring up the spreadsheet.
To enter numbers directly click on a box, enter the number and press RETURN. Once all the data has been entered click on all the rows and columns which contain the data to be plotted (hold the left mouse down and sweep through the rows and columns. This would display all these cells in the pressed down position.). Now click on the XY Plot icon (second icon) and the plot should be displayed in a Results window.
Instead of typing in the data it is also possible to read the data from an ascii file. To do that click on the Read File icon (first icon). Alternatively click on File and select Read Data... menu option.
In the new form select the ascii file from the File List and then click on the OK button. This should read the data and display it on the spreadsheet.
________________________________________
18. Troubleshooting
Q18.1 : In opening an existing PATRAN database the heartbeat continues to flash red indefinitely. What is the problem?
PATRAN has become a runaway process. See the answer to the question Q2.6.
________________________________________
Q18.2 : In submitting a ABAQUS analysis there is no *.fil file created. What do I do?
See also the answer to the question QX.X.
Check the contents of the nohup.out file. Usually ABAQUS messages are appended to this file, so look towards the end of the file and also check the date and time of the messages. There might be clues to the reason why the *.fil file was not created. If errors have been encountered in the run the nohup.out file might point to the *.msg or *.dat file for further clues.
Also look for the latest PATRAN message file. This will have the same first name as the PATRAN database but will have the extension .msg. followed by a number made of up of 2 digits.
Example : plate.msg.01.
Whenever a ABAQUS analysis is submitted or results are read into the PATRAN database a new message file with is created where the digits which make up the last extension is incremented by 1. For example if the newest file is plate.msg.n then if you submit an ABAQUS job the report of the creation of the input file will be placed in the file plate.msg.n+1. If the run was successful and the results are read back into the PATRAN database the report of that will be written to a a new file called plate.msg.n+2.
The sequence of events are as follows :
1.        The report from the creation of the *.inp file is written to analysis-id.msg.n+1. analysis-id.inp file is also created.
2.        The ABAQUS analysis is run. First the pre-stage and this is followed by the analysis stage. The report of these runs is appended to the nohup.out file.
3.        The *.dat, *.fil, *.msg files are created as part of step 2 above.
4.        One or more of these files will be missing if errors are encountered. If the errors occurred during the pre-stage then the *.msg file might be missing. If during the analysis the disk quota is exceeded the files *.dat and *.fil could be incomplete. See answer to the question X.X to verify if the problem was due to the quota being exceeded.
5.        The results are read back into PATRAN. The report of this will be written to a new file called analysis-id.msg.n+2.
________________________________________

[ 本帖最后由 yejet 于 2006-9-12 10:55 编辑 ]

stuartgew 发表于 2006-6-14 11:10

本帖最后由 wdhd 于 2016-3-23 14:25 编辑

　　好资料怎么没人看呢

　　下载下看一下就知道怎么样了啊

　　的确很不错的

xiaofang 发表于 2006-6-17 23:18

谢谢

wlxmkm 发表于 2006-7-6 09:36

thanks!

SEER11 发表于 2006-8-23 20:11

虽然是E文，但真的是不错。

redsky688 发表于 2006-8-23 21:59

谢谢

marybao 发表于 2006-8-24 09:29

确实挺不错的！

marybao 发表于 2006-8-24 09:29

确实挺不错的！

qhzm 发表于 2006-11-23 09:46

全是英文的阿，看起来有点费劲阿！

hfutbxq 发表于 2006-11-23 14:12

呵呵,谢谢,好东东

哲达武士 发表于 2006-11-23 22:59

好贴

GoldLily 发表于 2007-1-4 09:34

回复 #1 stuartgew 的帖子

本人刚开始学习patran，好好学习一下，谢谢楼主

查看完整版本: [共享］The MSC＿PATRAN FAQ转自剑桥工学院