How to show my 3D meshes in the window which feappv generates？

[wjs]

Dear Prof. Taylor/ FEAP admin/users of feappv:
  I'm using feappv to do some research.Some questions as follows bother me and I always feel helpless.
  1. I use the marco instrustions to generate the 3D mesh,but,when I run it ,the output in the window of feappv is just in 2d.I had tried many ways to fix it,then failed.So how to show a 3d mesh
in the window?The input file is as follows.
  2. I have seen the examples of FEAP and run some of them,but failed.And I just found one simple example in the website of feappv.Then I read the manual of feappv to study how to use feappv to simulate and do some reseach.However, it's two times I have read that PDF and I still have questions about how to make an input file.So do you have some examples especially in the aspect of J2 plasticity and coupled thermo-mechanical? I really need some help in this respect.
  Can you help me or give me some suggestion?
  Thanks a lot.

[Prof. R.L. Taylor]

Your input file has no boundary conditions.  It has a load.  Solving plasticity problems requires you to do an incremental loading which starts with several elastic steps before any yielding.  Also, you must be careful not to do too large of a plastic step at any time.  Incremental loading is done as a time stepping process.  You use loops and TIME commands setting DT to the increment you want to do.

Secondly, FEAPpv probably does not do any thermo-mechanical process -- in fact, FEAP does not have any thermal dependency in yielding behavior.  These are cases you will need to code yourself.

Displaying 3-d meshes requires use of PLOT PERSpective (and probably PLOT HIDE) to see what the mesh looks like.

[wjs]

Dear Prof. Taylor/ FEAP admin/users of feappv:
  Thank you for your quick reply, which makes me very surprise and exciting.
  With your suggestion, I have solved how to show the 3d mesh in the screen.I feel guilty about I didn't read the manual of feappv deeply,although it is hard for me to learn it well.
  To follow your advise, I just did some work today.Some questions happened(some of which existed long time ago ),then I am eager for your help again.The input file is as follows.
  1. I used loops and TIME commands setting DT to the increment, but I  did not set prop loading, and the force nodal condition is set(for example,1000N).So in the each time step,how the force loads,which means,does  the  force of 1000N load in each time step or does the force of (1000N/time step number) loads in each time step?
  2. I found some differences about  the unit of parameters. For example,what the uint of yield stress in feappv?    MPa or Pa?
  3. When I debug the program, I found feappv use the sld3d1() function in 3d calculation. The note in this function says  it is a "3-D linear elastic displacment element for feap".However, in this function, the program calls the function of plasticty(modlsd(),and then call mises() ) .I feel cunfused about it.
  4. I have read the output file after the feappv runs. Some expression I did not uderstand, like
  "*WARNING* sign of diagonal changed when reducing    3 equations."
  and
  " *WARNING* Lost at least 7 digits in reducing diagonals of    4 equations." Can you explain a little?
  5.  Whether the input files as follows call the suitable functions of plasticity?Is any mistakes in them?
  6. When I debug the program, I found it has three models(displacement model,mixed model and enhance strain model), I do not quite understand the latter two.Can you give me come ways to learn it well?
  Can you help me or give me some suggestion again?
  Thanks a lot.

[Prof. R.L. Taylor]

1. Forces will be nodal value times proportional loading function value.

2. feap and feappv do not have any units.  You must specify all data in consistent units.

3. yes feappv only has sld3d1, which is not very good for plasticity with large plastic strains.

4. these warnings warn you that you have rigid body modes in the model, for example you only have z restraints in the 3-d mesh, so x and y directions have rigid body modes.  You must resist rotations and translations in all direcrtions.

5. see above

6. our book (Zienkiewicz and Taylor and Zhu describe the element forms).  You can Google the types and probably find descriptions too.

[wjs]

Dear Prof. Taylor/ FEAP admin/users of feappv:
  Thank you for your quickly reply again!
  I did some work this weekend and still want some help of you.
  1.In your first reply, do you mean that even FEAP do not include the contents of problems about  thermal process such as creep and so on? Because I am doing some research about the welding simulation(more specifically,the constitutive models) with the FEM, so I must consider the effect of temperature. As a beginner, I really want you  give me some advice.
  2.When using feappv, if I want to input a complicated mesh in 3D,how could I do?
  3.Is the function of sld3d1()  good for plasticity with small plastic strains? Whether it will appear some errors(if my parameters right),and in what situations? In other words, whether the return map method works well in most cases,including different element,different constitutive model and so on.
  4.A small question:One element has four gauss integration points and one or two of them yield and others do not. Will this situation happen?
  5.My final input file is as follows.Is still some errors in it?And Whether it is a suitable calculation example of plasticity in Mises?
  I am just an abecedarian in such problems, so the question above may be immaturity. Therefore I need your help.
  Thanks a lot!

[Prof. R.L. Taylor]

1. feap does not support full thermo-mechanical behavior in the current release.  Probably will in the next release.
2. there are some mesh generation programs available.  depending on what you want to generate will help you decide which to try. do a search on the internet.
3. sld3d1 may not behave correctly when near incompressible behavior occurs.  mises plasticity with small hardening can cause this when plastic strains are larger than the elastic ones.
4. yes some gauss points may yield and others not.
5. you need to test this yourself.

in general you should read some literature on plasticity problems.  there are books such as the one by Hughes and Simo, or the one by Zienkiewicz et.al. on structures and solids, on inelastic behavior and element behavior. 

[wjs]

Dear Prof. Taylor/ FEAP admin/users of feappv:
  Thanks you very much!
  I will try my best to work it well.
  I wish Merry Christmas.