Creo Elements and Welding (FEM)

[Ignicolist]

Hallo,

I'm mechanical engineer and I work with Creo Elements (and Pro Mechanica) for FE calculations.

Now I would like to include in some of my calculations welded connections, but I fond some issues.
I can introduce the weldings, with the addecuate thickness and material, howeve, i can't understand the results.
To clarify that, I used the easiest example I can imagine:
- One plate is fixed (1). Welded to this fixed plate, I have another plate (2). At the end of plate 2, I introduce a force (down).

In the pictures, everything can be easily understood.
In picture 1, the complete structure.

The problem appear on picture 2 and 3. I dont kown where I should check for max. stress (that limits my welding). I this result, the highest stress can be seen in picture 2, inside the plate.

I would really aprreaciate if someone could help me, or orientate me with that.

Thanks in advance!

 

[shaun8567]

If you look at image "2" that you posted, you'll see that you welds look like rectangles with no thickness. This is because you've model the welds with shell elements (I assume you used Pro/Weld to define fillet welds, then used the "Weld Feature" part of the weld tool in Mechanica to create the weld. We can get into all the specifics if you want to, but the short version of it is that this is not a realistic representation of a welded connection, but rather a simplified model. This method is really used just to help distribute loads out a little more uniformly (compared to having bonded interface between the faying surfaces), but stress results at the weld won't be terrible accurate, since you're linking shell elements to solid elements.

A more realistic model would be to do everything with 3D solid elements (i.e. model the geometry of the weld itself), but at the end of the day, this would still be an approximation. For example, this model would not capture thermal expansion that happens during the welding process, the phase change that happens in the material during welding, the depth of the weld, etc. You COULD captures some of these by carrying out a transient thermal analysis that is then coupled to a non-linear structural analysis, but now we're getting into some pretty complicated physics/modeling.

 

[Ignicolist]

Thanks for your answer. I have checked and you are absolutelly right: there is no thickness and the results are far from the reality. Of corse, I used Pro/Weld and I see that this is not suitable for this calculation.

I updated my model with 3D solid elements to simulate welds. I enclose a picture of one of this modeles. Now the results seems to be more realistic than before, but once again I find an issue:
In the connection between weld and steel plate, I find some stress concentrations. You can find them also in the enclosed picture.
I tried different solutions, like using rounded weldings and I see that this stress concentration decreases.
Is there any "moro or less" realistic way to make welding calculations?
I made these calculation by hand and, where the structure has no deformation results seem to be possitive. However, in the areas where the deformation is important, stress in FEM is (much) higher than in my hand calculations.

I would like to use this weld calculation in an structure that is quite complicated (regarding these deformations), and I find nearly impossible to achieve a good result only by hand. Any idea is very appreciated to solve this structure.

Thanks in advance

 

[shaun8567]

The stress concentration issues you're experiencing is something innate to the finite element method called singularities. There are several different conditions that can cause singular results, one of which is a reentrant corner (such as the 90 deg corner created with a T-joint), and the stress results in singular areas will increase towards infinite as you refine the mesh. The effect of the singularity can be reduced by increasing the angle of the corner (an angle of 120 is considered a soft-singularity), which is what you've done with the addition of the weld geometry. Adding in a fillet further helps, but you'll never entirely eliminate it.

The way to handle a singular area (in Mechanica) is to add in a localized mesh refinement where the singularity occurs, followed by an additional layer of mesh refinement to act as "insulating" elements, and then use the mesh control "Isolate for Exclusion". This mesh control tells the engine to ignore the stress results on selected elements from convergence consideration, which is very important when one is after accurate results.

I threw together a very quick model of a T-joint showing the general thought process and took two screen shots. The "Volume Regions" image shows the two regions created for each part; the inner region should be large enough to allow the stress results to "smooth out" (think along the line of Saint-Venant's Principle), and the outer region is there to provide an insulating layer of elements between the singular elements and the elements you don't want to exclude. The "Isolating Elements" image shows the elements that have been excluded in red. All that being said, proper meshing to handle singular results is almost an art, and there isn't any real set of rules that will define all cases; you'll have to play around to find what works.

Another point/question I have is how you're handling contact between components and the welds. Are you modeling the structure with (1) connections between faying surface at the T-joint and between the welds, with (2) just the welds, or with (3) the welds and a sub-region of the faying surface between the T-joint? (1) is typically over-estimating the stiffness and strength of the joint (unless there is deep weld penetration), (2) is typically conservative (it assumes no weld penetration), and (3) is the closest to reality (but it assumes you'll know the penetration depth). You could use any of the three options in Mechanica (although with the third option you'll need to make some geometry modifications), so you'll need to decide how in-depth you want to go.

All that being said, what stresses are you calculating by hand? How are you modeling you screws? I noticed that you pointed out that if you remove a screw, then the stresses at point A increase; this seems correct as the load path through the screws closest to point A will end up carrying a larger load.

 

[uriel2k]

hello,shaun8567

I am a user of pro-mechanica for a long time. I was reading this thread, i am curious to know how you "insulating" the model with volume région (i use region volume often). You have writed:

"The way to handle a singular area (in Mechanica) is to add in a localized mesh refinement where the singularity occurs, followed by an additional layer of mesh refinement to act as "insulating" elements, and then use the mesh control "Isolate for Exclusion". This mesh control tells the engine to ignore the stress results on selected elements from convergence consideration, which is very important when one is after accurate results."

You tell us that u 've posted some image, but we cannot see them !

"I threw together a very quick model of a T-joint showing the general thought process and took two screen shots. The "Volume Regions" image shows the two regions created for each part; the inner region should be large enough to allow the stress results to "smooth out" (think along the line of Saint-Venant's Principle), and the outer region is there to provide an insulating layer of elements between the singular elements and the elements you don't want to exclude. The "Isolating Elements" image shows the elements that have been excluded in red. All that being said, proper meshing to handle singular results is almost an art, and there isn't any real set of rules that will define all cases; you'll have to play around to find what works."

Could you explain more about your technique, and post the pictures u told about to explain better ?
Hope you read this post and reply to me.

Thanks by advance.