Too Many Surfaces in Algor/Superdraw. 1

[toys19]

Hi,
I have recently been having problems meshing in Algor v19.3.
I'm new to Algor.
My 2 part assmebly will mesh fine in cad editor. Then in the fea editor I have been adding some truss elements and having to remesh and it doesnt mesh.... I think this is to do with the fact that the remesher uses the superdraw mesher to mesh and it reacts differently to the geometry..
Anyway sometimes I can get over that but then I come across the problem that the remsher has messed with my surfaces because it can only cope with 256 surfaces, so surface 257 merges with surface 1 etc.
Anyone know how to get around these problems?
Thanks
Toys19

 

[GBor]

You have 257 surfaces in a single part?

Any way you can show us your geometry? Take a look at the FAQ's for eng-tips (not the ones specific to this forum) to find places to upload files for free or for embedding a graphic in your post (usually not recommended).

Also, why are you having to remesh when adding the truss elements? Is there a way you can impose a break in your part so that you have an edge at the location where you are adding the truss elements? If you turn it in to another part in your CAD program, it should also cause your surfaces to renumber for each part, so it would reduce the number of surfaces in a single part.

 

[toys19]

Hi, sorry client confidentiality stops me from showing part.
Needless to say it has about 500 surfaces, its a complex injection moulded part with lots of ribs and ridges.
I have reduced the part geometry down through symmetry and de-featuring..
The truss elements are applied at normals to the part surfaces to simulate a one way boundary condition, like contact but without the contact, so the surfaces are covered in little hairs, which are trusses, the free ends have fixed boundary conditions, the other ends are connected to the surface. The truss has a stress strain curve which makes the stress very high for compression and very low for tension, hence the surface can pull away and stretch the truss, but cannot compress the truss. This simulates contact with an immovable object, neccesary for my analysis.
The truss elements are created by copying surfaces, offseting them from the surface and joining them, then the new surfaces are deleted, leaving behind the orginal surface and truss elements sticking out. After this the model requires remeshing in algor. Unless you know of a better, fast way of creating these elements on my many surfaces.
Its a pain in the neck becasue in Ansys you can set up a compression only boundary condition by slecting surfaces and ticking abox, it takes about 30 seconds, this method takes about a day for my model....

 

[GBor]

If you are using a curve truss element, is this a non-linear analysis? If so, right click somewhere off the model (but in the modeling window) and input an impact wall.

 

[toys19]

GBor,
Thanks for your rapid response.
Yep it is non linear.
This looks interesting, but let me explain further. The contact areas of my object are embedded in another object, the other object is of a very hard material, compared to the polymer the first object is made of. But there is no bonding between them, so when the polymer object is loaded I want it to be able to deform inside its restricted space.
I'm not sure how to use this function and they help file is a bit minimal.
So if I apply 6 impact planes all at 0.01 mm, will they effectively wrap around my object? Or will they be 0.01mm away from the furthest extremes of my object?
Thanks again
L

 

[toys19]

Hi Again,
Actually on reflection I dont think I see this working, I only want certain parts of my model to be restricted? Will it restrict the whole of my model?
Thanks
Toys19

 

[GBor]

It will restrict the entire model. Actually, though, it now sounds like you have more of a surface-to-surface contact issue. Let me just try to put some perspective to make sure I am understanding properly. You basically have something like a ball-bearing in it's cavity. You want to transfer the load of the bearing into it's cavity wall but allow it to move freely within the cavity. If this is the case, you want surface to surface contact. Otherwise, I'm still not understanding.

If it is surface to surface contact, then you will need to know what surfaces you want to contact each other. As the surfaces approach the contact distance, load is transferred between the two surfaces. It isn't quite as easy to set up as the impact planes because you have to establish the contact pairs, but it is still much more efficient than creating your truss elements and remeshing. Surface-to-Surface contact does not require your nodes to precisely line up.

As for the impact planes, the location is relative to the global coordinate system origin. So, an impact plane at 0.01mm as the "z roof" will impact all parts of your model crossing the plane located 0.01mm above the X-Y plane of the global coordinate system. Basically, you can define a box around your model and allow a ball to bounce around inside...

 

[toys19]

Thank for your help.
Trying to avoid setting up s-s contact in algor as it is really, really time consuming for this many surfaces.
Its not like a ball bearing its like a very complex PVC geometry, with 50 percent of it embedded in concrete.
I could just fix all the surfaces embedded in the concrete, but that would not be realistic, the contact surfaces need to be able to neck away from the concrete as the item is put under tension. So intially the parts are in contact, contact distance is zero, any surfaces that lose contact are due to the thinning of the polymer under tension (poissions ratio etc).
s-s contact would solve it really well but is computationally expensive. Also having tried it for this component, I have found that after 22 hours it gets to about 50% complete and then cannot converge. So I tried the truss method, which is quicker to set up and in theory should be much much quicker to run (remember I've got 500 surface about 300 of which are embedded).
Even if I could get the contact to work I dont want to use it if it takes 22 or more hours to solve, I want to to be able to do lots of runs to do mesh convergence studies, materials studies, load placement studies etcetc. When I set this model up with the contact surfaces just fixed and delete the concrete part - it solves in about 45 minutes. Secondly I have tried the truss method on simpler geometry which will remesh and has less than 256 surfaces and it works really well when compared to contact and gives the same results. For example a surface mounted (nylon) load point, bolted to a steel frame, as its loaded the contact flange deforms a bit and pulls away from the frame in places. When I modelled this s-s contact it took about 6 hours to solve and only after lots of goes to solve convegrence issues, basically you constrain it heavily in other area. When I solved this model with the truss method, solution in 25 minutes, first time. I'm not anti contact, but sometimes its not neccesary and time consuming.
So after setting up my trusses I have 2 problems- 1) I need to remesh and the remesher cannot deal with the geom as well as the intial mesher, 2) it runs out of surfaces - which redistributes any surface based loads and bc that are on the component, and makes it impossible to sort out, and impossible to adjust the model as you go along...
Any suggestions would be really welcome.
Thanks
Toys19

 

[GBor]

OK, one last shot. Have you considered building a third part out of bricks and giving them the curve properties much like you were doing for the truss elements? If you built this in to your CAD model, it should surface match both your "PVC" and your "CONCRETE". You could use any of a variety of material models, but I would think that a viscoelastic model or Ogden might work (treat your third part as a type of soft rubber or even an adhesive in reverse).

 

[toys19]

Gbor,
D'you know I think thats a really good idea, I shall give it a bash and get back to you with the results, thanks for all your input.
L