But Fabricio, I gave you a mesh with two elements through the thickness, I hoped you would use that.
I tried to use, but I need a refinement meshing in the hole region, because the contact between plate and washers. So I did the slice in the plate in this region.
In your model the are two elements through the thickness, but It was automatically. In my model, it does not happen automatically, I do not why.
In the hole region now it is ok.
What do you think?
How can I divide in two or three elements through the thickness if automaticall, it does not happen for me?
The attached archive has a boolean on some solids of the base of the beam, and added Sweep method on the base of the beam that specifies how many elements through the thickness of the base, and an inflation mesh control on the hole that specifies how many elements to inflate around the hole. I said 7 elements, but that is probably too many.
Check the material assignments!
The nodes between the beam and plate are not together, linked or merged. Is there any problem?
We started the discussion because this...
Peter, now I am getting confused, because the nodes are not corresponding...
Peter, I tried again with your model. But I think that you do not understand, or I did not understand. Your model is not possible to run, becasue the contact between the washers and the plates, the plate area, which you configure contact is so big. And the inflation, you do not separe the plate area in smaller faces.
Another point, we started the discussion, because you said that the pick stress in the beam was occuring becasue there were elements the I was not seeing, that I have to link the beam elements and the plat elements. And in your model it doesn't occur. It is not clear for me.
Sorry, but it is so difficult for me, because I am studying Ansys modelling for the first time. Thank you for being comprehensive with me.
Can you explain better?I tried again to turn the nodes between beam and plate coincident, but it does not happen.
I tried with boolean, I tried with your model, I tried slicing all the solids (that become extremely difficult to sweep small solids). The best meshing that I have reached is below with some comments.
So I try came back and use edge size through the thickness plate. Just see:
Ok it divides. But the nodes between beam and plate are different. So I am thinking to come back to my first model. The master thesis example is attached. The model too.
Please, can you help me again?In the other softwares are the same problem with the mesh. The people, normally use other softwares as truegrid to do the mesh. I think that Ansys should have a good mesh that take true result to compare with the reality.
As you se the picture below, the elements thtrough the beam length are not necessary, I need a refine mesh in the contact and where I apply the load. SO because this, I use edge size in the beam length with bias 10.
Can you point where I am wrong, PLEASE?
Here I did a resume:
1 - The elements in contact, beam and plate, have to be linked or not?
2 - How can I divide small elements through the thickness plate if using sweep it is impossible?
3 - The square, that male contact with washers is parametric, depending on the bolt diameter, so, for me is easy, it is linked with the parameters. So I am keen on using it. I have articles that explain it, and it is my reference in the master thesis. But they use truegrid to do the mesh.
4- What is the meaning of: "Solver pivot warnings or errors have been encountered during the solution. This is usually a result of an ill conditioned matrix possibly due to unreasonable material properties, an under constrained model, or contact related issues. Check results carefully."
5 - The peak stress in the results, is because the nodes that is not merged or near, or not?Because in your examples it does not.
6- Modelling beam and plate together, is necessary to create contact elements between them?
7- If I use slice in the plate or beam, I have to use contact between the solids created?
ANSYS can be very frustrating, because in one case, it shows its ability to form a perfect congruent mesh with hex element on the sliced solid with Shared Topology using no mesh controls, and then it fails to form a congruent mesh when some constraints are imposed on the mesh. I think the more bodies that are put into a multi-body part, the less likely the mesher is to form a congruent mesh. You can see why some people use 3rd party meshing software.
If you want hex elements, which you do, slicing is helpful to get hex shaped solids that can have 2, 3, 4 or more elements along edges. If the shared topology is working, then you don't have to do any extra work, as was the case in the 2 element example I provided above. When the shared topology fails, then you have a lot of extra work to do. You can put mesh controls on every edge of every block, set them to hard, and assign Face Meshing so that you get a congruent mesh.
1. For a study that includes large strain plasticity, you do not want contact elements to be in the plastic zone.
2. All the small bodies are sweepable so you can assign the number of divisions along the sweep.
3. Keep the slices around the bolt head as that is useful to you.
4. The meaning is one block is not merged with its neighbors. Add a Modal analysis to find if any pieces are not connected.
5. My examples were not ready for solving.
6. You do not want contact elements to connect the beam to the baseplate where they are welded together since this is where you are likely to see plasticity.
7. I don't know what you mean by splice.
1- I need contact elements, to simulate the beam and plate welded, no?Why not?If I don't use, there is a DOF.
2- But how I define along which edge it will sweep?
4 - It happens, I think because the number of slice that I am using, it is possible, isn't it?
5 - OK, but the mesh is important to solve.
6- Ok. But if I form a new part in the design modeler, is the same that beam and plate are welded, isn't it?
7- For example, if I slice a plate between to solids, when I go to the model, it will be 2 different solids in the same part. So it is not necessary to contact it, is it ok?
Thank you, very much!
1. Contact elements are useful in stitch welded structures to obtain the forces transmitted between members to evaluate weld stress with a hand calculation. If you are not doing a hand calculation of weld stress you don't need contact elements.
2. The sweep direction is specified after you choose a source face. The sweep direction is perpendicular to the source face.
4. Yes, I think one of the non-congruent blocks was not connected. A Modal would show that block flying out into space.
5. Once you get a good mesh, there is more work to get it to converge (after the Modal shows that it is connected).
6. Form New Part in DM is to weld the bodies together with Shared Topology. If that fails, then you have to do Node Merge.
7. When Shared Topology works, you don't need contact. When it fails, you do need contact or Node Merge.
I understand you are under a time crunch and I have time to help on Saturday.
Here is an example of using a Modal analysis to check if the mesh is connected.
You have to add the Fixed Support to the Modal system.
In this example, you can see that this body is not connected to its neighbors.
The corrective action is to make a named selection of all the bodies that are in that part, and create a Node Merge that merges the nodes in that group.
Once that is done, the Modal analysis gives a non-zero frequency.
Why should you have to do so much work just because the mesher doesn't do it's job is a good question.
Now the Static Structural model solves. Note: I had to set all materials to Structural Steel to have Modal run.
Yes, I think that I am doing all the mesh again, the Shared Topology does not work, and I have to use contact or node merge again.
So the result are the same which I have reached, I am trying again here...
Fabrico, I moved your reply to a new discussion because this thread was getting too long (Show More Posts).
I'm glad you have mastered the slicing and mesh controls and mesh edits needed to do this job. It's frustrating for me too.
I have downloaded your model and it is solving now. I will comment on your last post in the new thread.
Ansys customers with active commercial software licenses can access the
customer portal and submit support questions. You will need your active account number to register.