Welding assembly analysis

[JKI_PARTHIBAN]

Hi friends
I am going to a analyses steel plates assembly made of welding.... I have no Idea how to do it in Mechanica?
1.Is weld feature is enough to apply my sub-components or both weld and contact interface features should assign for my components?
2.If i am going to contact analysis I should need to assign Contact Interface to my components ?
please anybody guide me

 

[srieger]

A weld feature is nothing but a representation. You need to use a weld connection in Mechanica.

 

[shaun8567]

Pro/Weld (or whatever they are calling it) features can be used to create welds within Mechanica. I forget which version of Mechanica they introduced this feature in, but there is an option for "Weld Feature" (other options are "End Weld", "Perimeter Weld", and "Spot Weld"). However, this might not be the best way to go about your analysis; that will depend on what kind of results you are looking to get out of it.

Only assign contact interfaces if you're trying to model: (1) parts coming into contact that are not initially in contact, (2) parts that are initially in contact but are allowed to separate or slide relative to one another, or (3) if you need to know whether the frictional force between two surfaces is enough to prevent sliding.

Do you have a model you can post (either CAD files or just images) and more detail about the resutls you're after?

 

[Ignicolist]

Hello,

I have similar issue while modeling and analisyng welds in Pro Mechanica. I would really appreciate is someone could orient me in this matter.
To clarify this issue, I use a very simple assemble. You can find thins information under the following webpage.
Mechanical engineering other topics - Creo Elements and Welding (FEM)

Thanks in advance!

 

[shaun8567]

Hello,

I have similar issue while modeling and analisyng welds in Pro Mechanica. I would really appreciate is someone could orient me in this matter.
To clarify this issue, I use a very simple assemble. You can find thins information under the following webpage.
Mechanical engineering other topics - Creo Elements and Welding (FEM)

Thanks in advance!

In response to your question over at Eng-Tips:

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]

In response to your question over at Eng-Tips:

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.

Thanks for the answer. I check what you say and I see that you are right. Updated calculation can be found under this link:
Mechanical engineering other topics - Creo Elements and Welding (FEM)

 

[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.