Turn solid from step to shell in Mecway

leebailong

Hi everyone,
I am beginner in FEA.
I want to use step file to make geometry in MW. I have a problem because when I mesh my model, MW is making two parallel mesh connected up and down. I want to have only one mesh. Cen you help me?

Victor

Mecway doesn't do midplane extraction from solids. Some alternatives:

• Using the surface mesh you have, delete the extra surfaces, leaving only one. Use Edit -> Edge detecting selection to easily select large curved surfaces. If the offset from the midplane is a problem, you can then define a Shell offset in Element properties.
  
• In your CAD program, make the geometry only a surface instead of a solid.
  

An unrelated point. Turn on Fit midside nodes to geometry in Meshing parameters otherwise the curves become faceted and stresses will be less accurate.

leebailong

Thanks for reply.
I was make the geometry only a surface in Ironcad. In internal solver evertything was ok, but in CCX I had again two mesh. Look at the pic, this is the same model in different analysis. In internal solver i had 676 nodes, but in CCX 1586.
In static 3d results are almost equal, but in buckling 3d the diference is very big.

prop_design

that's normal for ccx. it expands the shells into solid elements. Make sure to set the element orientation, if using composites.

For ccx, use the following cards, if using composites:

*EL FILE,GLOBAL=NO
S

Also, for ccx composites, add 'don't generate keyword' *EL File

There's an option to change the shell offset also. You should probably check to make sure that ccx expanded the solids the way you expected. You can move it around with the offset option.

Update; I downloaded your model. I see it's very thin. So it's hard to see the shell expansion ccx does. But it looks like it expanded about the midplane.

My experience with the mecway shells is not to use them. They are more like plate elements. For your curved cylinder, i would be surprised if they work right. Visually, the ccx results look good. I switched your model to nonlinear and ran it. It looked good as well.

disla

In general, when solving buckling you need a mesh size capable to capture the size of the smallest wave pattern. Here , mesh size is too rough to capture it and results are not accurate in any of the two solvers in my opinion. Try a thickness of 20mm and ccx which solution has a more reasonable number of waves for your mesh to see what I am talking about.
For such a problem solution should be some kind of regular deformation pattern which can also guide you to discard bad solutions, imperfections in your mesh or any other pathology.

prop_design

i've never did a buckling analysis. but i noticed your material doesn't have density defined. for modal analysis, density is important. not sure if this is an issue in your case or not. also, the shell offset option is in element properties. so if you select all your elements and then click element properties you can change how the solid expansion is done. i imagine it works for mecway shells too, but never tried that. if you read in the manual, it mentions the mecway shells shouldn't be used for curved geometry. some slight curvature is ok. but based on your stress plot, i would say to stick with ccx in this case.

prop_design

to disla's point. if you select all your elements you can go to mesh refine x2. i did that twice in a row and ran the model. it does look better. you have to update your saved node selections. but that's easy to do. the saved face selection seems to update on it's own. i attached the models i setup with these changes. but it's worth it to try yourself for practice. the modes are more refined, but having never did buckling analysis before, i'm not qualified to address that aspect of your question.

leebailong

prop_design
I'm intresting only in steel structures. If you say composites you mean plastic?
I don't read manual for Mecway, I don't know that I can't use internal solver for curved shells, thanks.

disla
I'm traing now free version so I can't use more nodes

My problem has a analytical solution

G = 0,605*E*t/r=0,605*210000*1/500=254MPa

a=254/50=5,08

You are close.

prop_design

hi,

by composites i meant orthotropic shell elements. something like carbon/epoxy. i hadn't looked at your model when i wrote that. for your original model using ccx linear i get 51.85 MPa. With the refined mesh using ccx nonlinear i get 55.48 MPa so not a big change. On the modes, I'm not sure if you need to specify density. I'm not sure how it even solved with it being blank. The modal analysis won't solve but the buckling does. So maybe victor can clarify how buckling solves without a density value. From the equations I looked at online, it seems to be the same formula where the mass matrix is used. In any event, the first non zero mode has a buckling factor of 27.117 with your model using the ccx solver. For the refined mesh it's 5.71, using the ccx solver, and the mode looks completely different. so i imagine for that analysis you need a more refined mesh, like disla said. i didn't know you were using the trial version. so that's why i posted the results here. this is for the 1mm thickness you had defined.

anthony

disla

Internal solver seems to solve pretty accurate once refined.
You can recognize clearly a pattern which is also a good sign.

Victor

A few comments:

You don't need density for buckling. Though the eigenvalue equation is similar to the one for vibration, it uses the geometric stiffness matrix obtained from stress instead of the mass matrix.

Curved shells are OK with the internal solver, especially gentle curves like this where the ratio of radius of curvature to thickness is high. Twisted shells are not very good though.

There's no need to use formulas for cylindrical coordinates in the displacement constraints here because they're equivalent to ordinary global x,y,z constraints and are probably getting replaced by them internally anyway. But there's no harm in it if you're planning to extend this to something more complex later.

The radius is 499.5 mm which I guess is an error due to using the mesh of one surface. You can change it to 500 mm using Mesh tools -> Node coordinates or with a 0.5 mm shell offset if it matters.

CCX solution decreases with refinement, hopefully towards 5.08.

Internal solver solution also decreases with refinement, below 5.08 to values like 5.05.

I guess if you know the number of waves around the circumference, you might be able to use a small segment of the cylinder and mirror symmetry to capture exactly one wave with a low node count. Kind of risky though because that's excluding many possible wrong solutions.

prop_design

thanks for the clarification victor. after i read your post i searched for a better form of the equation and it's clear now. i didn't understand the BC setup but left it alone. so i'm glad you clarified that as well. one thing i don't understand, the ccx solver seems to give a mode for a buckling factor of zero. i was just ignoring that. could you explain what that mode is and why it's there. with the internal solver you seem to have to guess at one of the settings. which makes it pretty weird for a newbie. i like that ccx seems to just output the results with no user guessing. if you have no idea what you are looking for, how would you get the internal solver to find things?

as far as the internal shell elements. to me, the ccx stress results look like what you would expect. even when i refine the mesh, the internal results are a little odd. even for this model. the contour plots look off some. as far as the stress magnitude, the results are pretty close to ccx though. i didn't do much with the modes, since you seemed to have to chicken peck at an input setup and then get modes out.

leebailong

What about shear locking? If CCX change quad8 into hex20 elements, we don"t have a problem with that?

Victor

The mode 0 seems to be the solution from the static analysis used to obtain the geometric stiffness matrix. I don't think it should really be there, but it might be helpful to confirm the loads are being applied correctly.

I agree that choosing the Shift point by trial and error is a pain. That seemed to be a requirement of the ARPACK solver but somehow CCX doesn't need it. I don't know if it determines it automatically or somehow avoids using it. If you have no idea of the buckling factor, you can still start with a small value like 0.00001. In this case, knowing the theoretical solution means you can just pick Shift point to be a little lower than that. I set it to 1 and just left it there.

Victor

I don't think there's any problem with shear locking. But in case of related issues, you can change to reduced integration. CCX -> custom element type, select Quad8 and enter S8R in the CCX element type box.

prop_design

hi,

perhaps this helps in your evaluation. ccx nonlinear was able to solve up to the buckling load factor of 5.7. a value of 6 wouldn't solve though. the stress plot is with a cut-plane, so you can see the high stress on the inside of the tube.

prop_design

i increased the mesh density another x2 and the buckling load factor is about 5.1. so it's closer to the theoretical. that load factor seems to correspond to the load limit for the ccx nonlinear solver. once you increase the load past that, it won't converge. i did some more tests, but no need to post results. pretty much the same as above.

barmin

Is there any info when (or if ever) CCX will have the true shell element? Becouse for shells this even reduced integration seems weird and I assume that shear locking will appear to some degree anyway.

Anyone with better shell experience in CCX can shed some light onto it?

prop_design

Since the step file wasn't uploaded, I didn't have many meshing options with your model. I took some measurements inside mecway to try and figure out the dims of your model. It looks like it was a dia of 1000mm and a height of 1000mm. So I made a new midplane step model, that way I could experiment more with meshing. The 1mm thickness was too thin to use solids. I manually made the mesh in mecway using quads. I also made a quad mesh with netgen. Both those meshes wouldn't do any post buckling deformation. It seems the misalignment of nodes, when using tets, allows the post buckling that I was seeing. For some reason, your original mesh, with a 3x x2 refinement also did post buckling. So the nodes must be a little misaligned there. The only problem is that is a much bigger mesh. It took over 2 hours to run. I worked on it for a long time to get the run times down. Some meshes wouldn't get good agreement on the buckling point. I compared the first buckling mode to what the nonlinear solver would show for the buckling load factor. I've attached a tet mesh that solves very fast, has good agreement, and shows the post buckling deformation. You can't run it with the trial version though. That only has a 1,000 node limit. The attached model has 5,844 nodes before the ccx expansion. Then it has 13,180 nodes. The 3x x2 refined mesh, that I started with, had 40,352 nodes before expansion and 94,224 nodes after expansion. I changed to fixed displacement at the base. This gives a different deformation shape, that matches what you see with solid models. Fixing x,y,z disp, with shells, seems to allow rotation. So the shape looks different than what you get with a solid model. The other bc are the same as what you specified, but done in a more simple manner.