FEA hotspot on filet

[Anonymous]

I modelled a part in 2013 and ran an FEA and got a hotspot on a filet. Refining the mesh made the hotspot a good bit worse. The high stresses dropped down tremendously very quickly. When Algor FEA'd the same part, same loads etc. it did not get a hotspot. A friend of mine has reported the same behavior and always on filets. Has anybody else noticed filets having strange results in FEA?

[JDMather]

Have you gone through Wasim Younis book?
Attach example Inventor and Algor files here.

[Anonymous]

Right now the best I can do are 2 jpegs of a similar FEA done at home. The problem FEA is at work. Tomorrow I will see what I can sneak out on a thumbdrive.

The FEA at work was of a truss joint. A 30 inch pipe, two 10 inch pipes and a plate. The joint was modelled in frame generator, an ipt was derived from the assemby and chamfers were added for the weld. (I'm hoping my memory is good.) The Von Mises stresses on the part at work were initially 680 ksi on a node 2/3 of the way up the filet. Maybe 3 nodes away the probe said the stress was 16 ksi. I split some faces and refined the mesh and then the stress jumped up to 980 ksi on a node that was again about 2/3 of the way up the filet. Maybe 3 nodes away the stress had again dropped to 16 ksi. I know that memory isn't what you want. You want the computer files. Like I said, I will see what I can sneak out of work.

The Inventor derived part was exported as a stp file to Algor. Algor's analysis didn't have hot nodes.

The FEA I just did at home isn't nearly as odd as the one at work. The hot node is at a corner instead of in the middle of the chamfer's flat face. It does cool off in a hurry.

I haven't read any books about FEA.

[Anonymous]

First I need to clear up some poor wording on my part. The hot spot is on a chamfer that acts as a fillet weld.

Second, I asked the boss if I could post a company file. Presently I can't but that may change tomorrow. The owner of the company is thinking about the benefits of learning something versus the secrecy. I can post a better screenshot than the ones I posted before.

The hotspot is on a corner. I was thinking it wasn't. And looking closely at the mesh shows an odd spacing of the nodes exactly where the hotspot happens to be. I expect that I need to learn how to massage the mesh to get more believeable results.

I don't have access to the Algor analysis. I don't know how much massaging of the mesh was done in Algor.

[Inv_kaos]

"I haven't read any books about FEA."  - Yet you are running FEA?.. FEA, like most engineering software, is garbage in = garbage out, so how do you know the results you are getting are accurate (hot spot or no hot spot).

This apparent peak stress is caused by a singularity at the sharp re-entrant corner. It is a fictitious stress that will increase infinitely as you refine your mesh. You should check for convergence to make sure that your stress away from any singularities is accurate - these stresses will converge but a singularity won't.

The difference between the software would only be due to discretisation of the mesh and the element types used. The theory (in those books  ) is the same. However if you have a choice of software i would use Algor over INVSIM.

[falkmassmann]

The problem is known, I think even by Autodesk. In general the FEA in Inventor is using poor meshing algorithms on Weldments and fillets if you don´t alter it to the specific area.

This is an exhausting task with Inventor since most of the time you will have to create surface cuts to apply a finer mesh in that specific area.

The problem is that the meshing is too coarse and sometimes it get´s reduced to just one triangle.

Imagine you extrapolate a fillet with just one triangle, if you apply torque to one of the three nodes it will calculate a way too high stress on just that one node because you´re running out of material in that node.

The only way to calculate that properly is a finer mesh which Inventor FEA doesn´t compute automatically.

I do FEA´s with weldment assemblies and I have that problem all the time, I´m just ignoring the hot spot´s because I know it´s not calculated properly.

For example in Ansys this is no problem at all, the mesh adapts to the stresses and geometry.

Unfortunately I can´t run simulations with Ansys all the time cause I´m sharing the license.

You might not have read books about FEA, but I guess you have knowledge about mechanics of materials which every Engineer worth its salt should have.

People will try to dissassemble you for saying that you have not read a book about FEA like the guy above.

Which doesn´t mean you have no knowledge in that area.

Cheers Falk

[Inv_kaos]

FEA is an engineering tool to be used by experienced analysts. If you refer to a quality assurance standards, like that in the pressure equipment industry and others, it is clearly stated for minimum requirements. I am not suggesting you can't learn how to do it but you should pick up a book and learn what is going on. Get Wasim Younis' book if nothing else.

Knowledge of mechanics of materials is good because you should be performing hand calculations to check your FEA results. You don't need to be able to write FEM code, just an understanding of how the inputs affect your output and how to validate and verify your results.

If you over stiffen your model, under refine your mesh, apply loads and boundary conditions incorrectly, etc, you can be out by 200% or more. As a design verifier I come across this regularly, I am not trying to disassemble anyone just encouraging them to do it right, no criticism intended.

Even with Algor the default mesh is coarse, you will need to refine it suitable for your model. Inventor allows this as well but with fewer options available to the user.

[Anonymous]

The owner of the company allowed me to bring home a weldment .iam and a derived .ipt home to mess with. The derived part was used because chamfers are quicker and easier to apply than fillet welds in a weldment assembly. The derived part is posted. Take a look at the chamfer.jpeg. There is a .00047 mistake in a chamfer. That .00047 jiggle is where the FEA mesh is crummy and that's where the hot spot occurs. The fillet weld command in the welding environment doesn't produce this .00047 problem.

I was going to attach a bunch of screenshoots but it appears I can only have three attachments. The last attachment will be the mesh done by Algor on the derived part with the .00047 jiggle in the chamfer.  The Algor mesh sure looks clean. None of the Inventor meshes looked anywhere near as clean and simple.

I think there is a problem with the chamfer command and Inventor's FEA meshes don't look too great either.

[Inv_kaos]

Don't forget you are comparing a Hex mesh to a Tet mesh, they will always have a different appearance. In this case a quadrilateral will fit a four edged face better than two triangles, particularly when skewed but generally tet elements will fit complex geometry better (might not look as good though). See attached for compariison of Inventor and Autodesk Simulation (Algor) tetrahedral mesh - they are quite similar. However they do have different meshing engines and Algor is pretty good for surface meshing (try not to look at the volume mesh).

The 'jiggle' is caused by the curved geometry since the length of the chord varies for the same leg size (but perhaps a developer could comment on whether it is an error).

I would suggest start by refining your global mesh in Inventor before you apply any local mesh refinement. This is partly what is causing your poor mesh appearance. Then apply your local mesh refinement to the areas of interest. You will get a better continuous mesh field and also better results. I always start by reducing my transition to 1.1 or 1.2 (sometimes less) and then play around with your average size and min size to suit.

As a general rule of thumb you can work on 2-3 elements through the thickness for membrane stress and 3-5 elements through the thickness for bending stress, to give good results. This can be reduces in areas that aren't of interest to your stress results but you should check this with convergence.

If you are after the maximum stress in the weld then treat the number of through thickness elements as through the weld throat. You wont be able to accurately measure the stress at the weld toe but you can use a geometry stress method to extrapolate the stress at this loacation. You can find such a method in most fatigue codes, such as DNV-RP-C203 Clause 4.3.8. This standard also has a lot of information on pipe to pipe joints and stress in welds, just like your geometry, that you might find useful. It is free online.

Hope it helps.

[Anonymous]

Your Inv mesh really looked good. I've copied and pasted your help into a document. I'll mess some more with the FEA stuff at home. I actually do 90% AutoCad at work. About the only Inventor work I do is when somebody can't do something. That's how I got involved with this FEA comparison of Inventor with other stress softwares. Thanks for all your help.