Register to reply

Mesh Convergence Issue In Ansys

by cemadenver
Tags: ansys, convergence, issue, mesh
Share this thread:
cemadenver
#1
Feb9-13, 05:02 PM
P: 4
Hi Guys,

I 'm currently trying to make a 2D model of a sector of a compressor disk with the blade attached to it by means of a frictional contact (as shown in the attached pic). The contact between the blade and disk is frictional (coeff=0.25), augmented lagrange formulation, and adjust to touch interface treatment. I subjected all bodies to rotational velocity of 1000rpm and the boundary conditions are friction-less supports at the bottom of the disk and at its two sides (which would represent the symmetry condition during operation of the full disc). I need to determine the equivalent von-mieses stress on the disk, just below the contact point of the blade and the disc. Now, my problem is that when I tried to do a mesh convergence test, von-mieses stress value at the point of interest does not reach a stable value as I refine the mesh. The error percentage from the previous mesh refinement run doesn't keep reducing. I'd be really grateful if anyone could help me around this.
Attached Thumbnails
dovetail pic.png  
Phys.Org News Partner Science news on Phys.org
Law changed to allow 'unlocking' cellphones
Microsoft sues Samsung alleging contract breach
Best evidence yet for coronal heating theory detected by NASA sounding rocket
cemadenver
#2
Feb9-13, 05:15 PM
P: 4
I just have one more request, I need to solve this issue in a very short time and it's quite urgent for me. Will be extremely grateful if someone can help me resolve this soon.
AlephZero
#3
Feb9-13, 07:00 PM
Engineering
Sci Advisor
HW Helper
Thanks
P: 6,967
Are these 4-node or 8-node elements? it's hard to tell from a small-scale plot. 8-node elements will probably behave better for the curved contact faces you have, if Ansys has an 8 node element with the analysis capabilities you want (I dont know, I'm not an Ansys user!)

I suspect the "random errors" are partly caused by the distorted element shapes around the small radii. Having all the elements about the same size in a model like this is fairly wasteful. You probably have 10 times more elements than you need over most of the disk sector, and 10 times too few where the stress field changes rapidly. Make sure the element shapes in the critical regions are as close to rectangles as possible.

This is a a more complcated geometry, but look at the mesh in Fig 3 and compare with yours. http://www.sciencedirect.com/science...68874X99000724

Or Fig 4 here: http://www.sciencedirect.com/science...42112312000400

cemadenver
#4
Feb9-13, 08:38 PM
P: 4
Mesh Convergence Issue In Ansys

Hi AlephZero,

Thanks for the quick response. I tried what you told me, mainly refining the mesh locally with quad elements (most are quad, though some sparse elements had to be triangular to satisfy continuity in some regions). However, I still don't think that mesh refinement is converging for me. I've posted a graph plotting iterations vs quantity. The iterations are in steps of 0.2 mm except the last three which are in steps of 0.03mm. I used the edge sizing method of workbench for the local mesh. The last mesh size I used was 0.11mm and I think it still didn't converge (as you can see in the graph). At this point I stopped because any further refinement in mesh wasn't helping, infact all quadilaterals couldn't be maintaned at that size and the mesher had to replace many by the more robust filling but less accurate triangles. I've read some papers on fe analysis of dovetail regions of turbine discs of a similar geometry and I don't think any of the papers had to go anywhere near 0.11mm for convergence. There is one thing I forgot to mention in my previous post, I have two error messages: "one or more contact regions contains a friction value greater than 0.2mm and an unsymmetric solver had to be used" and "one or more bodies may be under constrained and experiencing rigid body motion, weak spring have ben added...". I feel though the second message however is not abnormal since, I'm dealing with friciotnal contact and naturally there has to be some sliding. I've also attached the total deformation behaviour of the model just in case you want to have a look at that also. Thanks.
Attached Thumbnails
2D mesh refinement result.png   total deformation.png  
AlephZero
#5
Feb9-13, 10:28 PM
Engineering
Sci Advisor
HW Helper
Thanks
P: 6,967
If your displacement plot shows the actual movements (not scaled in some strange way) there is something unrealistic going on. The "blade" shouldn't be pulled a quarter of the way out of the slot. It's hard to see what has deformed wrongly from just one screen shot though.

Try a run where the blade is fixed into the disk (no sliding interfaces, just equate the matching nodes on the blade and the disk) to check you get sensible looking displacements and stresses.

Then, presumably, you can make a similar model with a very large coefficient of friction and get similar results. Then reduce the friction to the value you want.

"one or more bodies may be under constrained and experiencing rigid body motion, weak spring have ben added...". I feel though the second message however is not abnormal since, I'm dealing with friciotnal contact and naturally there has to be some sliding.
You said you had a frictionless constraint on the "bottom of the disk". If the bottom of the disk is a circle, that means it will be free to rotate about its axis, so the program will have to fix that up somehow to make the stiffness matrix nonsingular.

It might be better to fix it yourself, by constrainng one node to have zero circumferential displacement, rather than letting the program try to fix it aotomatically.

Depending how Ansys works, you may also need to fix the blade to the disk just for the first iteration, if something nonsensical happens at the start because there are no loads on the sliding boundaries.
cemadenver
#6
Feb9-13, 10:55 PM
P: 4
Hi AlephZero,

Thanks for the response. Just had a quick question, how will the disc rotate with a fixed support at its base? Thanks.


Register to reply

Related Discussions
Ansys Workbench Load Application Issue Mechanical Engineering 0
Mesh in Ansys problem Mechanical Engineering 0
ANSYS workbench 11 mesh help! Mechanical Engineering 25
Second Order Circuit Analysis - Mesh - Issue with DE Setup Engineering, Comp Sci, & Technology Homework 5
Issue with mesh analysis of 4 loop circuit Engineering, Comp Sci, & Technology Homework 0