Femap FAQ (English)

Femap is an application that is used to create finite element models and to analyze the results of calculations done with those models. It is a so-called pre-/postprocessor for finite element models. The analysis itself is not done by Femap, there must be another software (so-called solver) for that. Typically, Femap is used in conjunction with the solver NASTRAN. Femap is also a graphical user interface (GUI) for the solver. Femap exists since 1985, and currently it is in the software portfolio of the Siemens branch “Siemens Digital Industries Software”. For more introductory information see the Wikipedia page of Femap.

01. What does “`PREPROCESSOR CONTROL VALIDATION FAILED.`” mean?

The reason is most probably special characters in the input file. When the file checksum is calculated Femap and NASTRAN treat special characters differently, and this is where the error comes from. This also applies to entity names, because these are written as comments into the DAT file and comments are part of the checksum calculation.

02. What does “`USER FATAL MESSAGE 9002`” mean?

Spaces in the model name, spaces in the path to the model file, spaces in the path to Femap. Special characters, like ä are also forbidden in path and file name.

03. How can I make Femap output the min and max values of the front- and backside of plate elements combined?

In Model/Output/Envelope chose From Output Set, and select the appropriate output set. As Vector select Plate Top and Plate Bot and then a new output set with min and max values will be generated.

04. How can I show the min and max values over all layers of a laminate?

See “How can I make Femap output the max and min values of front- and backside of plate elements combined?”

05. What is shown on the X-axis of XY-diagrams?

Under View/Select chose one of the following options:

Option                       x-Axis
======                       =======
XY vs ID                     ID
XY vs Set Output             Set ID
XY vs Set Value              Output Set Name
XY vs Position               Position along one of the axis
XY vs Function Value

06. What are the different function types good for?

Function types and their usage:
Generic
1. Dimensionless
16. Function vs Value — multiple curves associated with a given quantity

Dynamic
2. vs Time — time dependent loads for transient analysis
4. vs Frequency — frequency dependent loads for frequency response analysis
7. Viscous Damping vs Frequency — damping for transient/frequency response analysis
8. Critical Damping vs Frequency — damping for transient/frequency response analysis
9. Amplification vs Frequency — damping for transient/frequency response analysis
17. Function vs Critical Damping — tables obtained for/from Response Spectrum analysis

Nonlinear
3. vs Temperature — temperature dependent material properties
5. vs Stress — stress dependent curves for nonlinear material properties
6. Function vs Temperature — multiple stress/strain curves as a function of strain rate for nonlinear material properties
10. vs Strain Rate — yield stress as function of strain rate for nonlinear material properties
11. Function vs Strain Rate — multiple stress/strain curves as a function of strain rate for nonlinear material properties
14. Stress vs Strain — stress/strain curve for nonlinear material properties
15. Stress vs Plastic Strain — stress/strain curve for nonlinear material properties for export to those analysis codes that require input in plastic strain
12. vs Curve Length — define load magnitude as a function of curve length
13. vs Parametric Length — define load magnitude as a function of parametric length

07. What entities are there in Femap?

Coordinate System
Point
Curve
Surface
Solid/Volume
Text
Boundary
Node
Element
Material
Property
Load Set
Constraint Set
View
Output Set
Output Format

08. How can I find out more about functions like `XEL()` or `SIN()`?

Appendix C of the User Guide has a Function Reference.

09. How can I change the background color of a window?

By a click of the right mouse button on the window title bar you can change the window's properties, like for example the background color.

10. The title bar of my window has disappeared. How can I get it back?

Shift and right mouse button brings back the title bar.

11. The small `Dynamic Query` windows don't disappear. How can I get rid of them?

The little windows that appear when you leave the mouse pointer on a node or element for a while are called Dynamic Query Window in Femap. Sometimes they stay stuck on the screen and don't disappear automatically. To get rid of them, do: Delete/Tools/Text and then select all the windows you want to delete. See also: “How can I get information about a certain node or element quickly?”

12. How can I get information about a certain node or element quickly?

On the right side of the status bar select the Entity you would want to show. Move you mouse pointer over the element you want to query and leave it there. A small window with selected info is shown. Which info is shown depends on the selected Output Set and the selected Output Vector. This functionality is referred as Dynamic Query in the manual. Other useful functions are: Dynamic Query + left mouse button copies text in the List Window Dynamic Query + right mouse button copies text in the Graphic Window To view the test, it must be in the current Group and the screen must be redrawn.

13. Which cards are produced for temperature related settings?

Model/Load Body/Default Temperature TEMPD Model/Load/Body/Reference Temperature (is not actually written) Model/Material/Reference Temperature MAT1 Model/Material/Functions/Reference Temperature TABLEM2

14. How much does Femap cost? [Removed, because the answer was outdated]

15. How much does similar FEM software cost? [Removed, because the answer was outdated]

16. How to calculate a response spectrum?


DLOAD -> RLOAD1 or RLOAD2
RLOAD1 -> DAREA -> LSEQ -> LOAD
METHOD Refid
EIGRL Refid

Cards that are used for the response spectrum calculation.


LSEQ Loadset <-> DAREA
RLOAD2 DAREA
PLOAD4
DLOAD scales RLOAD2
TABLED1	TID	XAXIS	YAXIS	XY ... Loads
TABDMP1	TID	TYPE	XY	XY ... Modal Damping
LSEQ	SID	DAREA	LID
RLOAD2	SID	DAREA	DELAY	DPHASE	TB
PLOAD4	SID	EID	P1

DLOAD
FREQ	SID	F1
FREQ3	SID	F1	F2	TYPE	NEF

17. My View isn't shown, but it is activated?

First minimize and then maximize the Femap window. The View is then shown minimized within the Femap window.

18. How to activate the writing of `F06`, `XDB` and `OP2` files?

A PARAM,POST,-1 statememt activates the writing of OP2 files
A PARAM,POST,0 statement activates the writing of XDB files
A PARAM,POST,1 statement activates the writing of F06 files

Among the output statements in the Case Control Section there must be PRINT.
For example:
DISPLACEMENT(PRINT)=ALL
In the document Result-Destination-Summary there is an overview of the possible options.
In Femap the output type is chosen in the NASTRAN Case Control Dialog.
The dialog is available under File/Export.../Advanced or File/Analyze/Advanced and OK.
In newer versions of Femap it is under Model/Analysis in Analysis Set of the Output Request Dialog.
You can choose from:
Print Only: The output will be written into a F06 file.
PostProcess Only: The output will be written into a OP2 file.
Print and PostProcess: The output will be written into the F06 and the OP2 files.
Punch Only: The output will be written into the PCH file.
Punch and PostProcess: The output will be written into the PCH and the OP2 file.

19. How to set the orientation of a material?

For 2D-elements the material orientation can be set under Property Type/Material Orientation. The orientation can be defined with nodes, a vector, a coordinate system or an angle. (Model/Property.../Elem/Property Type.../Element Material Orientation) (Modify/Update Elements/Material Angle...)

For volume elements a coordinate system can be set at the assigned property. (Model/Property.../Elem/Property Type.../Solid/OK/Material Axes) The coordinate system must already be defined. Alternatively the material can be defined with the axis that go through the nodes.

For line elements it is possible to define an element orientation. (Modify/Update Elements/Orientation...)
(Model/Element/Type.../Bar/OK/Orientation)

20. Check Coincident Elements doesn't find existing coincident elements?

If you click a mouse button while a coincident element check is running the check will be cancelled. Existing coincident elements are possibly missed. Whether the mouse is clicked within Femap or outside it doesn't matter. An indication of the completion of the check is that the mouse pointer returns to its normal pointer form by itself. However, it does so too when the check is cancelled by mouse click. In case no coincident elements are found the completion of the check is also indicated by a message “No Coincident Elements Found.”.

21. What do `MAXRATIO` and `BAILOUT` do?

PARAM,MAXRATIO, This value is the threshold for the ratio between matrix diagonal and factor diagonal.
A setting of PARAM,MAXRATIO,1.E+8 is the standard default value.
When the value of MAXRATIO is exceeded, the value of BAILOUT determines what happens.
With PARAM,BAILOUT,0 NASTRAN will cancel the analysis run when the threshold is crossed.
With PARAM,BAILOUT,-1 crossing the MAXRATIO
threshold is ignored.

22. How can I change the coordinate system that the `Dynamic Query` (Tooltip) shows?

In Tools/Parameters you can choose the active coordinate system. This coordinate system is used for the data in Dynamic Query.

23. How to make images for Microsoft Word?

You can create images for word either as bitmap or vector graphics. Each has advantages and disadvantages.
Here is how you can create a bitmap graphic:

In Femap

Turn on render mode
Ctrl + C

In Word

Paste Special
As Device Independent Bitmap

Sadly it is not possible to select a custom resolution for the bitmap. “File/Page Setup/Render Res Factor” does not work as it should.
A vector image can be made like this:

In Femap

Turn render mode off
Ctrl + C

In Word

Paste Special
As Picture

Sadly this does also export hidden polygons, so that the vector file can get very big.

24. How does a CSV file for Femap have to be formatted?

See CSV-Format.pdf

25. How to create `RBE2` and `RBE3` Elements?

NASTRAN RBE elements are called “Rigid Elements” in Femap. If an RBE2 or an RBE3 element is produced depends on the presence of an interpolation factor in Femap.

RBE2: rigid = no Factor
RBE3: interpolation = with Factor

There is always one independent node and several dependent ones.

     indy
     /|\
    / | \
   /  |  \
 dep dep dep

Rigid elements are used to

model areas that are very stiff compared to the adjoining structure in order to prevent numerical difficulties and often to simplify the model
used to connect two coincident nodes that have different coordinate systems

RBE3 spider (e.g. for bolts)

123 123 123
 \   |   /
  \  |  /
   \ | /
   123456
    /|\
   / | \
  /  |  \
123 123 123

26. My laminates are too thin.

Most probably they are not. If the checkbox “Symmetric Layers” in Define Property - LAMINATE Elements is checked, NASTRAN uses twice the specified thickness for analysis. Femap will show the specified thickness though.

27. I need a node with two different output coordinate systems.

A node can only have one output coordinate system. What you can do is to create two coincident nodes, each with its own output coordinate system, and connect them with an RBE2 element. A connection with RBE3 seems to work, but it is not entirely clear from the documentation if this is supported. CELAS do not work here, because they require both nodes to be in the same coordinate system.

28. When I display a deformed model, the deformation is in the “wrong” direction.

Using a scale factor of -1 for display is unfortunately not possible. As a workaround you can multiply an output set or an output vector with -1. You will create a new set or vector that you can plot. Do it like this:
Model/Output/Process/
Linear
Scale Factor -1.
From Output Set select
To Output Set select
Add Operation
Another way is to animate the model and create the screenshot in the right moment.

29. How can I let NASTRAN show the used `MAT` cards.

All MAT8 cards (2D Orthotropic) are transformed into MAT2 cards by NASTRAN. It can be useful to have these MAT2 cards and use them for example for plate elements that are laminates. To make NASTRAN output the MAT2 cards it uses internally, use a
NASTRAN PRTPCOMP=1
statement at the beginning of the bulk file. You can enter this in Femap in “Model/Analysis/NASTRAN Executive and Solution Options” under “Start Text”. For current (~2006) NASTRAN versions this is enough, the MAT2 cards will be written as INFORMATION MESSAGE to the F06 file. For older NASTRAN versions (for example those included in Femap) you need to additionally specify ECHO=PUNCH Model/Analysis/Output Requests/Echo Model


ECHO=PUNCH

The MAT2 cards can then be found, together with the PSHELL cards, in the Punch (PCH) file.

30. Can I have a temperature gradient between front- and backside of plate elements?

Sure, but unfortunately not in Femap directly. The required NASTRAN card is TEMPP1. In order to enter one of these via Femap you have to create a dummy temperature load case first. You then have to assign a temperature to an arbitrary node. Then you can enter the card manually under Model/Analysis/NASTRAN Bulk Data Options/Start For example:


$2345678 2345678 2345678 2345678 2345678 2345678
TEMPP1         6       1     0.0     0.4
               2    THRU    5000

Caution: Femap uses a proportional font in this dialog, which makes the manual entry nearly impossible. It is better to write the card in a text editor and then copy it into Femap.

31. How can I create a temperature gradient?

Model/Load/Nodal/Temperature Method Variable !!!! Temperature dependent on coordinate Then enter (xnd(!i), ynd(!i), znd(!i)) as equation. It will not work if you forget to click “Method Variable”!

32. Where does the information in this FAQ come from?

This is a summary of my notes from the years 2000 to 2006, when I was working full-time with Femap and NASTRAN.