Input file problem

[mohany]

I have another model built in ANSYS workbench, using remote nodal displacement. In the input file from ANSYS, there are about 20k nodes and around 10k element. I want to paraphrase them in FEAP form, but there are so many lines, Are there any quick method to solve my question.
I will attach my and FEAP input file (Still fixing) in this post, if someone has some way to overcome this "stupid" problem, I would be grateful for that.

Best

(Idrawing is the FEAP input file)

[mohany]

I update my input file, but there is still error shows:
     *ERROR* MESHCK: Data for material set    0 on element       3600 not input
Note: The following floating-point exceptions are signalling: IEEE_DIVIDE_BY_ZERO

But I do check the input file, I don't think there is mistake. Could someone correct me on this input file?

Thank you

[Prof. S. Govindjee]

You are getting closer. 

The first problem, which I have fixed for you, is that there can only be 16 items on a FEAP line, further items need to be on the next line.  See section 5.2.2 of the manual.  It was easy to fix the problem with an AWK script.  See the attached file.  Which has a few other fixes/suggestions

The next thing you have to is to fix your boundary conditions.  See the manual for what is needed.  Also be aware that solid elements in FEAP have only 3 DOFs per node so you only need x,y,z boundary conditions.

[mohany]

Thank you very much, Professor Govindjee.

I will get back to this post once I have further questions regarding this.

Best regards
Mohan Yu

[mohany]

I have modified the FEAP input file, But I still get error show below:
"   Energy convergence test
    Initial   =    0.000000000000000E+00 Current   =    0.000000000000000E+00
    Relative  =    1.000000000000000E+00 Tolerance =    1.000000000000000E-16"

I think it might because of the material property does not define properly. However, I have checked the material property of the input file, I cannot find some problem. Could someone help me to clarify this problem.

Input file attached at here.

Thank you very much

[FEAP_Admin]

You are not applying any boundary loads.

In FEAP this is a two step process.

1.  Set the BOUNdary codes to a non-zero value on dofs where you will apply displacements.

2.  Use the FORCe command to set non-zero force values on dofs with forces (boundary code should be zero for these dofs).  Use the DISPplacement command to set non-zero displacement values on dofs with imposed displacements (boundary codes should be non-zero for these dofs).

Right now you are not applying any non-zero forces or displacements.

I also recommend using OPTI to reduce the size of your profile to speed up the solve.

[mohany]

In my case, I am trying to analyze a displacement-driven problem, there is no force load on that.
Could I only have the boundary condition with fixed dof, and the displacement?

[Prof. R.L. Taylor]

Yes, you need to specify BOUN and Disp for all the driver docs.  There are several options for these, such as EDIS or CDIS.

I BELIEVE YOU HAD THE LIST IN YOUR ORIGINAL MESH BOT IN A DIFFERENT INPUT FORM

[FEAP_Admin]

Example.  Suppose you wish to apply ux=0.1 to node 1 and uy=0.2 to node 2 and ux=uy=0.3 to node 3.  Then you would need the following lines

Code: [Select]

BOUNdary
1 0  1 0
2 0  0 1
3 0  1 1

DISPlacement
1 0 0.1 0
2 0 0    0.2
3 0 0.3 0.3
Only the displacement values where the boundary codes are non-zero get used.  The others are just ignored.  See the manual for other ways to specify boundary codes and displacement values.  [If boundary codes are zero, then FEAP reads force values from the FORCed command etc.]

[mohany]

I see what you are trying to explain. Thank you!