Stress Analysis of Weldments In Inventor or Algor 1

[barrti]

HI,
I am using Inventor 2011 for FEA of welded structures. Generally it is ok unless I am interested in the stresses in the weld. I get a lot of stress singularities here.

I also have a number of issues when I try to model a flange that has been welded around its outside to another member or indeed, when I bolt the flange to the other member.

I usually change the bonded contact between the flange and other member (not the welded area) to "separation/no sliding" contact but I have had a number of doubtful results here.

I understand the limitations of Inventor, however the majority of my office uses it for drafting for which it is very powerful.

My questions are then:

-Is Autodesk Mechanical Simulation (Algor)a good alternative?
-Will it give valid results near the welds?
-Is it easy to transfer a model to it from Inventor or am I better off with a different FEA package?
-Does anyone have experience using Inventor for welds?

 

[GregLocock]

I'm giving you a star for asking the right questions, and the horrible answer is that Inventor is a fine tool for generating solid models, but for complex FEA you need to look elsewhere once you have your geometry.



Cheers

Greg Locock


New here? Try reading these, they might help FAQ731-376

http://eng-tips.com/market.cfm?

 

[barrti]

Thanks Greg, I was starting to think that.

 

[rollupswx]

-Is it easy to transfer a model to it from Inventor...

This doesn't make sense.
Inventor is a modeling software.
Autodesk Simulation (formerly Algor) is an analysis software.

You don't transfer a model from Algor to Inventor - you go the other way around. You transfer Inventor models to Algor.
You model in Inventor and analyze the model in Algor.
After installing Algor there is a tool in Inventor to click to go directly into Algor with the model. Any changes (within reason) made in Inventor are updated in Algor.

 

[rollupswx]

Oops, I read the original post wrong.
But I think I answered the question.

 

[EngAddict]

barrti, response to your 4 questions.

Part 1:
Yes, Autodesk Simulation (ASM) is much better than Inventor Simulation. Inventor can be used for basic simulation and optimisation but you are very limited by features, most of which are required to competently conduct FEA and generate reports for professional use. So while a designer could use Inventor to roughly design a part, I would not recommend to use it for the engineering design.

For example I was supplied with a part from another engineer who had a designer at another company questioning why we were saying his part was failing (just as it was about to go into production). Basically the problem was a designer using a tool designed for engineers and lack of training in setting up a simulation. Also the contact options and post processing tools hindered his ability to adequately validate his design. I could go on about the limitations but essentially if you know what you are doing you can use Inventor for some simple simulation work with accurate results . Adding 'thin elements' or whatever they have called shell elements will be a big advantage for Inventor. Why they don't incorporate more plassotech features, I don't know.. but it was a very capable program.

Part 2:
A singularity is a singularity, basic FEM theory and doesn't matter what software you are using. You are best to use averaged stress methods across the weld but if you refine the mesh sufficiently and/or linearise the stress through the weld throat, then you can get accurate local stress results (won't be able to linearise in Inventor though). Just remember to make sure you refine the mesh until you get convergence and don't take stress probes at a singularity and a sufficient distance away from stress intensifiers. If you are doing fatigue then that is a whole other post. However you can use a 'geometric stress' method that essentially smooths your stress result and omits the peak component of your stress so you can get the accurate total stress at the edge of the weld (would work well with the limited features in Inventor).

Part 3:
You can click the add in button in Inventor or open it directly through ASM. However you can also do this for many other leading CAD packages because Algor was previously not owned by Autodesk but also still supports the other packages. One advantage you have with Inventor is that you can directly manipulate Inventor parameters in ASM which you can't do in the other programs.

Part 4:
Yes, do you have any specific requirements? Like are you only interested in adding strength to your whole model with the weld included or is it a specific analysis of the weld itself?

Algor is a very good program but I am not overly impressed with its volume meshing capability. Has a very good surface mesher though. Maybe also look into Femap with a Nastran variety or Abaqus, Comsol would also be worth a look. Most FEA packages support all major CAD packages but AFAIK ASM is the only one that has the Inventor parameter link. Still though, nothing beats the ability of Soliworks to model and simulate quickly, then modify your design and re-run without losing simulation input. However SolidWorks simulation is still more limited than the other packages I listed but can handle just about any type of work in the right hands.

Sorry for the essay, I hate long posts..

 

[barrti]

Engaddict, thanks for your post. Re part4. I need to look at the strength of the weld i.e. I need to look at the fatigue life and strength of welded structures. Many times, the weld area is highly stressed so I need to accurately model the weld itself as well as use appropriate contact elements under any un-welded areas.

Today, I obtained the triaxial stresses from Inventor for a fillet weld. I'm manually calculating shear stress in the weld throat as Inventor doesn't quite give that. I will then use this with a structural code. The application I'm thinking of is not a high risk one however, its apparent that we have exceeded Inventor's capabilities!

Part of the problem with Inventor is that it only has tet elements and is linear so stress singularities occur as the mesh is refined around the weld..often convergence does not occur. I'm getting better at ignoring some of the stress singularities but I worry that, sometimes I am ignoring real problem stresses. I suppose the answer here is that If convergence has not occurred then we have a genuine stress singularity.

What do you mean by "However you can use a 'geometric stress' method"? Can this be done within Inventor?

 

[EngAddict]

If your stress converges at a 'reasonable' distance away from the singularity/intensifier then your stress converges. It is very unlikely you will want to be running non-linear for fatigue analysis. It mostly depends on what fatigue code you are working to. Do you have access to PD5500 or AS1210? If not refer to ABS, the link is below, on page 14 they have what is called 'Stress Gradients (Actual & Idealized) Near a Weld'. DNV also have a similar method called 'derived target hot spot' search for DNV-RP-C203. If you are using a structural stress method or working to ASME VIII then you will be outside the capability of Inventor (without stress sections or linearisation). ABS and DNV are available free online and are very similar to PD5500 Annex C which is probably the best of the fatigue codes. The applicability and the validity of the structural stress method is debatable, i.e. still not universally accepted among the experts in the field.

http://www.eagle.org/eagleExternalP...gueAssessmentofOffshoreStructures/Pub115_FAOS

 

[barrti]

EngAddict,
thanks, those links are very helpful, I need to read them more thoroughly and look for a more capable fea application.