Hi everyone,
I am trying to do the 2-step simulation for pre-stretch structure.
Step1: I apply the displacement as the boundary for static analysis to get the pre-stretch. It is succeed. Then I change the Step1.rout into Step2.rin file.
Step2: I give a load along the y direction on surfaces. After finishing the simulation, I check results and find that results are the same with the Step1.
My setup files are shown in this link GitHub - NUGUY2022/2step_simulation.
I want to get some helps. Thank you!
- Why aren’t you using membrane elements instead of solid ones to model the membrane ?
- Restart is not really needed here, you could just run a 2 step analysis.
- What’s up with those keywords ?
*BOUNDARY,FIXED
**INCLUDE,INPUT=Solid/boundary-restart.inp
**BOUNDARY,OP=NEW
*Nfix1,1,1,0
*Nfix1,2,2,0
*Nfix1,3,3,0
Is this whole section supposed to be commented out ?
Q1: Why aren’t you using membrane elements instead of solid ones to model the membrane ?
I don’t know how to use the membrane elements now. So I want to test the 2-step simulation firstly.
Q2：Restart is not really needed here, you could just run a 2 step analysis.
I write this setup file according to others. Does “restart” have influence on this simulation?
Q3: What’s up with those keywords ?
I finish the step1 and get the step1.frd file. Then I run step2 and get the step2.frd file. When I check these two files in PrePoMax, I find their displacement is the same. It makes me confused because I give a constant load 10 along the y direction on the surface. I’d like to know why the displacement in step2.frd is the same with step1.frd.
Q4: I write this section to fix the low boundary. I think it can’t be commented out.
No but it’s more convenient to run a 2-step analysis instead (in this case).
I think that the section I pasted above is causing the issue here. Try changing it to:
*BOUNDARY,OP=NEW
Nfix1,1,1,0
Nfix1,2,2,0
Nfix1,3,3,0
This will remove the boundary conditions from the first step and only redefine the listed ones.
I change this section into
*BOUNDARY,OP=NEW
Nfix1,1,1,0
Nfix1,2,2,0
Nfix1,3,3,0
The low boundary is not fixed. The membrane is moving along the y direction.
Is it still with restart ? I tested this using a single input file with 2 steps and it seems to be working fine.
My 2-step simulation want to realize this situation.
- The membrane is stretched under the hydrostatic pressure.
- The membrane is deformed by dynamic forces.
Did I write the right setup files?
I think your pictures show a good result. I also use Restart. I am a fresh man of calculix. So I don’t know how to make a 2-step file into one file. Can you give me an example?
You can just copy the contents of the second input file to the first one and remove the *RESTART keywords. So there should be something like this:
*STEP
*STATIC
...
*END STEP
*STEP
*DYNAMIC
...
*END STEP
Step.inp (920 Bytes)
I use this setup file. I can’t get results in your pictures. Is there somewhere wrong?
You have:
*BOUNDARY,OP=NEW
*Nfix1,1,1,0
*Nfix1,2,2,0
*Nfix1,3,3,0
while it should be:
*BOUNDARY,OP=NEW
Nfix1,1,1,0
Nfix1,2,2,0
Nfix1,3,3,0
CalculiX should throw an error message that *Nfix is not a valid keyword (Abaqus does that) but, unfortunately, it just ignores this.
You are right. I can also do it by two files. The main problem is
*BOUNDARY,OP=NEW
*Nfix1,1,1,0
*Nfix1,2,2,0
*Nfix1,3,3,0
After I remove " * ", it works. Thank you so much.
So sorry to disturb you again.
A friend mentioned me that there is a little difference between the final displacement in Step1 and the initial displacement in Step2, when I do it by two files.
Step1.inp (532 Bytes)
Step2.inp (397 Bytes)
Maximum final displacement of Step1 = 1.31mm
Maximum Initial displacement of Step2 = 1.14 mm
Let’s just continue the topic on the CalculiX forum, no need to duplicate it here 
Are you Calc_em? I don’t know this situation. 
So sorry about that.
Yeah, that’s me No problem at all 
Thank you so much. You help me a lot.
1 Like