[C_O]

Hello friends;

This is my first thread on this forum. Hi to yours all.

I am working at the automobile industry for design engineer. And working for AnSys analysis generally.

Nowadays, I am working different types of meshing operations. I am trying to reach o-grid type of mesh on the cylindrcal profile. But this is not the linear profile, it is circular, like coil spring (automobile front or rear spring)

Could you give me some help about this process?

All your thinkings will appreciate.

Best regards.

[PSYMN]

If you use the Ogrid tool (in ICEM CFD Hexa) or use Multizone with inflation in ANSYS Meshing (same underling ICEM CFD hexa Ogrid code), it will handle it for you.

In interactive blocking, you just block out the tube with a rectangular block wrapped from end to end... Add splits along the way and fit the rectangular cross section to the model... Then add an OGrid. Select all the blocks, add faces to the ends and hit apply... It will take care of the rest.

If you are using multizone, it does the blocking for you. You just need to set the method for that body as "Multizone" and put a named selection on the side of the spring (not the ends) so you can apply inflation. Then hit generate mesh. If the surface structure is not condusive to Multizone, you may be more successful by "splitting" the spring a number of times across its length... Either at the surface only or the bodies (but make it a single multibody part).

[PSYMN]

If your spring has many turns, it may be good to use a sub model... Just block a single turn and then use blocking topology options to copy it up the rest of the way.

[Vidyanand Kesti]

If you are meshing ANSYS mesher best you can slice the model at each turn and at the end of the face you can slice the model to get the o-Grid,but its time consuming and its depend upon the number of turns

[C_O]

Thank you friends. I think, I will handle it with your opinios. I will back to you after my works on it.

Thanx again.

[C_O]

Hello friends, I hope you are doing fantastic.

I am working on my model for meshing with o-grid type. Actually I made some steps.

You can follow the attachments like 1 and 2.

3 is my full-model.

I think I have done it about %70.. But problem is not sweeping mesh with all bodies. For example, you can see in 1.jpg, all plane meshs are same. but in the other parts of model are not. you can see in 2.jpg. Right side different, left side different.

I sliced my model as you suggest. you can follow it on 3.jpg and applied all parts multizone by one by. of course with named selection.

Could you help me for this problem...

Thank you by now.

[C_O]

There is no opinion for this? I really need your suggestions..

Thank you very much and have nice day.

[jrunsten]

Did you use "Multizone" as your mesh method in Ansys meshing? Or just Sweep?

On the other hand.. Have you created a single Part from your bodies in DesignModeler?

[PSYMN]

Originally Posted by jrunsten

Have you created a single Part from your bodies in DesignModeler?

Yea, I think the issue is that you have separate parts instead of a multi-body part.

You should select all your parts in DM and right click to form a new part... The mesher will then know to give you a conformal mesh on the multi-body part.