Simulation Mechanical Forums (Read-Only)
Welcome to Autodesk’s Simulation Mechanical Forums. Share your knowledge, ask questions, and explore popular Simulation Mechanical topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 
Reply
Message 1 of 16
bjorn_fallqvist
618 Views, 15 Replies

Using spot welds

Hello,

 

I am curious if someone here has an idea of what I am trying to do;

 

I have two overlapping sheets of metal (surfaces modelled with plate elements). If I wish to create a bolt between these two to find out the shear force between them, is there any way to model a zero-length beam element or something similar to do this? Unfortunately the surfaces are made in the same plane, and of the same thickness (due to some CAD-constraints). I was thinking of simply using spot welds instead to do this somehow, but I can't find any such option in Algor.

 

Any suggestions?

 

Much appreciated

Björn

15 REPLIES 15
Message 2 of 16
S.LI
in reply to: bjorn_fallqvist

I'm trying to understand your problem correctly.

"overlapping" is to connect bottom surface of part A and top surface of part B, right?

If yes, there should be a gap between shell element mesh, since shell element is generated on mid-plane from CAD.

So it's OK for you to have nonzero length beam elements over there.

 

 

----------------------------------------------------------------------------------------------
If this response answers your concern, please mark it as "solved".
Message 3 of 16

Hi,

 

This may be a bit non-practical, but I'm trying to find a way to do this without offsetting the shell/plate elements or modifying the CAD-model. Is there something like "beam offset", but for shell elements instead that allows you to position the elements in the same plane and then use offsets to make the FEA pre-processor create MPC constraints between them? I know you can do it with tied contact in the MES, but is there a similar thing in the linear solver?

 

I guess using manual MPCs may be one way to do it.

Message 4 of 16
xli
Alumni
in reply to: bjorn_fallqvist

Björn,

 

Currently we don't have shell (called plate in LSS) with offset support similar to beam's offset. User manual specified MPC allows almost doing anything to such connection. But it looks only feasiblly for tiny simple models as you seen. We are also on the way making support to automatic connection between solid and shell element, which automatically make MPCs for given structures. But it will need user's configuring of the connection, e.g. welding connected (some MPC needed), simply-connected (no MPC needed), shell covering solid, ... 

 

I am not very clear what you want and what configuration your plate model is. A simple figure would have been helpful. There is a function in fea editor, under geometry:add:contact elements (manual). That can manually making contacts. I am not sure if this can be useful for your case or not? just an idea.

 

Also if you provide a little bit more details of your case and waht connection you would like to make automatically, it may help us to consider a better implementation supporting solid-shell case as well as some special shell-shell case too. Thanks you very much.

 

-xli

 

Message 5 of 16
S.LI
in reply to: bjorn_fallqvist

I'm not talking about offset.

Let me step-by-step understand your problem.

 

1.) You have parts in a CAD model

2.) for one or more parts, you want to mesh it/them into shell elements

3.) select midplane (instead of plate/shell), since plate/shell method will generate a empty box based on the CAD surfaces.

 

4.) is there gap between shell-mesh parts?

 

thanks.

----------------------------------------------------------------------------------------------
If this response answers your concern, please mark it as "solved".
Message 6 of 16

Hi,

 

The real problem is that we have a client who does sheet metal constructions (silos and the like) in which the sheets of metal bolted to eachother are overlapping in the CAD-model, and they are reluctant to change the way they build these models. That's why I was thinking that maybe there was something similar to offsetting them from eachother.So the surfaces are in the same plane.

 

The goal would be to try and find the shear force in the bolts around the circumference. I guess it could be made by splitting the two surfaces (for example one a hexagon and the other a square) around the bolt holes, then creating spokes, moving the center node a little bit out in the normal direction of the surface, drawing a bolt and rotating the lines. But that has caused me some trouble with the mesh of the two surfaces matching (something I don't want since the lines snap to the nodes on the opposite surface when I rotate them) even though I say they shouldn't. I'm guessing this is because they are in the same plane.

 

It seems that there are a lot of bolts around the circumference though, so maybe the easiest way is then to just have everything bonded and look at the local stresses at a cut plane instead.

 

Thanks,

Björn

 

Message 7 of 16

Speaking of which, how is the stiffness matrix affected if we have several bonded plate parts in the same plane? Are there contributions to the respective nodes' degrees of freedom from each element? It seems reasonable to me that the membrane stiffness contributions should be the same (representing a plate of twice the thickness), but what happens with the bending contributions?

 

Thanks,

Björn

Message 8 of 16
S.LI
in reply to: bjorn_fallqvist

I think the true bolts are not necessary to be simulated in your problem.

What you need is just the constrain at the bolt hole for overlapping sheets.

Then the local stress should be good enough.

 

My suggestion is to apply constrains along bolt hole edges based on shell element meshes.

1.) it could be bonded directly if meshes on two part are matched at the bolt hole

2.) otherwise, you can try smartbonding in LSS

 

 

----------------------------------------------------------------------------------------------
If this response answers your concern, please mark it as "solved".
Message 9 of 16
S.LI
in reply to: bjorn_fallqvist


@bjorn_fallqvist wrote:

Speaking of which, how is the stiffness matrix affected if we have several bonded plate parts in the same plane? Are there contributions to the respective nodes' degrees of freedom from each element? It seems reasonable to me that the membrane stiffness contributions should be the same (representing a plate of twice the thickness), but what happens with the bending contributions?

 

Thanks,

Björn


About stiffness matrix, if it's directly bonded (common nodes), the contribution should go to the same DOF. If the meshes are not matched exactly, kinds of MPCs are used. (I'm not clear the details in codes).

----------------------------------------------------------------------------------------------
If this response answers your concern, please mark it as "solved".
Message 10 of 16
bjorn_fallqvist
in reply to: S.LI

Ok...I have another question now; how can I ensure that the meshes do not match if the plates are in the same plate? I have ensured that the "Do not match meshes" under model mesh settings is turned on, but it still snaps the nodes together.

Message 11 of 16
S.LI
in reply to: bjorn_fallqvist

Do you mean "do not match the mesh of the contact pairs"? This is another story for more accurate results in surface-to-surface contact applications. It's not suitable for your case.

 

I don't have a way to guarantee non-matched meshes. But my suggestion is to adjust mesh size part by part to avoid the common nodes. In the treeview, for each part, there is "CAD Mesh Option", right-click, and select "part", then you are allowed to change the setting for individual part.

 

----------------------------------------------------------------------------------------------
If this response answers your concern, please mark it as "solved".
Message 12 of 16
bjorn_fallqvist
in reply to: S.LI

Yes, but shouldn't it also ensure that the meshes don't match generally?

 

How does adjusting mesh size avoid common nodes? Even if one part has a smaller mesh size, the program will snap them together...

Message 13 of 16

Hi Bjorn,

Wow, forget about the FEA, there is a lot of engineering things going on in this model. I love it!

You have probably thought about these aspects, but I will mention them for everyone's benefit.

  1. You said that the plates are in the same plane, mainly because of how the CAD model was created. How confident are you that neglecting the offset is acceptable? In real life, a membrane force in the plates will cause bending at the overlapping joint. I was thinking about scaling one of the shells radially to put the plate elements at the proper midplane. Of course, if the shell has stiffener ribs, then these ribs would be scaled also, making them a slightly different size.
  2. In real life, the plates are connected through the bolts (or spot welds) but also make contact between the two overlapping surfaces. Are you including the contact? If so, then you want the meshes to match, and you eliminate one of the problems!

The attached figure shows one suggestion for how to make a "bolt" or "spot weld" between two plates that lie in the same plane (courtesy of Joe S. and I). This method requires the meshes to not match. So, the answer to your question of how to make the meshes not match.

  • Make sure that surface knitting is turned off when you are importing the model. ("Tools > Options > CAD Import > Global CAD Import Options")
  • Select the two parts that you do not want to match (or two surfaces), right-click in the canvas, and choose "Contact > Free". (This is the trick that you were looking for!)
  • As you mentioned in one of the posts, the "Model Mesh Settings > Options > Model > Do not match the mesh of contact pairs when applicable" needs to be checked.

This will not force the meshes to match. Or you can think of it as each part being meshed separately. However, this does not guarantee that a random node will not line up. In particular, if two parts have a corner at the same location, then you are guaranteed to have a node at that same location. But since the contact type is free, they will not be bonded! (The same is true with surface contact.)

 



John Holtz, P.E.

Global Product Support
Autodesk, Inc.


If not provided already, be sure to indicate the version of Inventor Nastran you are using!

"The knowledge you seek is at knowledge.autodesk.com" - Confucius 😉
Message 14 of 16

Hi, John

 

I know, it's one of the more non-FEA-related problems I've run into lately, for a change.

 

1. I am fairly certain that disregarding the offset is reasonable. We're talking about plates that are 1-2mm thick in a structure which has a diameter of several meters, so on the whole I don't think it's going to affect the results much.

 

2. Yes, I am including the contact, so I'm guessing the meshes should be matched for this purpose.

 

The real problem I have with this mesh matching situation is that when I create a pin joint, it works fine for one hole. But if I would need to sweep these lines to create the entire bolt pattern, the lines seem to snap to the nodes around the hole, making the entire area around the hole more or less bonded. I was hoping to avoid this by making sure the nodes around the holes do not match.

 

I really would like to change the basic way of drawing the CAD-model but this is in response to a customer who always draws their CAD-models this way and would like suggestions on how to use them in Algor.

 

Message 15 of 16
xli
Alumni
in reply to: S.LI

Hi Bjorn,

 

Thanks for the image of the CAD model that helped understanding of your model better. 

 

Here are a few modeling ideas I can have (may duplicate ideas people already talked in this thread):

 

(1) Solid model. It requires CAD model has no volume overlapping, so both parts as solid elements. They have connected surface and you may setup in various ways: surface contact, bonded (requiring matched mesh), smart bonding (called bonded contact now, requires MPC), or free surfaces + spot bolted. We can see such a solid model would be more close to the real world problems. However, as you have stated you cannot go this way. And model size is probably another strong reason you have to use shell element for thin structures.

 

(2) Since CAD model has to keep overlapped so that both parts will have to be modeled as shell element parts and in the same mid-plane. Bjorn, I remember you once had several shell parts overlapped in same mid-plane kind models before. You are an expert in this area. It may make things more complicated but also may give more opportunities to handle the problem in different ways: 

 

(2.1) If you are not really interested (or can ignore) the relative deformation between parts and localized deformation around bolts, then you may not have to use bolts. Make a fully bonded model. Then a potential problem is that two parts may not have a good matched mesh. Then some of those missed match will give not good solution. Besides adjusting mesh sizes in both parts to get better match, another idea is that you may cut overlapping section in CAD model as duplicated parts.

 

(2.2) Then you may have part 1 and part 2 shorter. And two new parts with same meshing geometry and eventually will have exact same mesh that is easy match for fully bonded model. And the stress in any of these parts in supposed bolts area give you a “rough” (or say averaged) results of what you are interested as you indicated early.

 

(2.3) If you are interested in the contact between parts and needs bolts, you need to set a contact pair of part1 and part2 as free/no contact. And then at those positions supposed to have bolts you can manually build up MPCs to tie nodes between two parts. The condition is where you have matched node pairs, and two nodes have equal DOFS (three translational DOFS or all six DOFS). It would be a time consuming operation :-(. But I suspect the current existing bolt wizard wont’ do good job in the case you have, which is shell-to-shell in same mid-plane. Because all those spokes of the bolt will be in the plane so that they are hardly to carry load normal to the mid-plane there (however, I might be wrong here since I have no experience of bolts, please correct me thanks).

 

There could be a way to better and flexibly make MPC connections between parts providing models similar to (2.1) and (2.2), As an answer to your previous question, then such model will same DOF or equivalent DOFs for both side’s elements. So in final matrix, they behavior like two sides are tied together there.

 

Bolt way is different mechanism. They use “rigid” spokes tie those nodes together and that is why require two sides have different nodes. I would see there is a problem in your case that all spokes in same plane. A bolt using MPCs instead of spokes would be a better solution for (2.3). But we don’t have it now. Manually building up them is just an idea, I don’t know practically you want to do or not. Thanks. 

 

-xli 

 

 

 

Message 16 of 16
bjorn_fallqvist
in reply to: S.LI

Thanks for the suggestions! I think the easiest way is to simply run the model bonded, then, since the client was looking into an easy and fast way of doing it. I was just wondering if there was any way to do it quickly and reasonably accurate. 🙂

 

By the way, I don't think I've used overlapping shell elements before? I do recall having had shell elements and edges of solid elements overlapping, though. In that part, I could get around the overlapping problem with offsetting the shell elements in the CAD model itself...wish I could do the same here. 😞

 

 

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report