Stress output for weld calculation

JRP

Does anyone have any sugestions for stress output for weld calculation. When I was using Ansys Mechanical APDL, I used path plot and there I was able to get stress output to calculate welds.
I know this is not possible in Mecway, but maybe there is some other way to get to something useful?

disla

Hi,

¿By path plot do you mean Stress Linearization.?

In that case this option is available in Mecway.

Go to the GUI Tree > Solution (Right Click) > New Stress Linearization.

JRP

Ok. I get it. Thanks for this. But if I understand corectlly this is only available with solid elements?
I have most of the models built from shell elements. I'm looking for something like that.

disla

You can do it with shells using ccx.

JRP

Ok. Thanks for this info. Unfortunately, I have some problems with type of elements and loads. If I use CCX, then I can't use line pressure on line3 elements.

Victor

Can you be more specific about what stress data you want? Can it be derived from the existing stress or bending moment data?

JRP

Let say that we have two plates welded toghether. Something similar as disla posted. I would like to get to normal and both shear stresses on the plates contact. With that I can specify the welds.

https://www.researchgate.net/figure/Level-of-stress-in-fillet-weld-a-calculation-thickness-of-weld-l-length-of-weld-3_fig1_265941993

https://www.ideastatica.com/support-center/fillet-weld-in-lap-joint

mmartin

Good afternoon JRP:

I enclose a 3d model involving weldings.
I know that this is not what you are asking for. However, I think you might find it usefull.

In this case, I phisically defined the welding and used "bonded contact" option to link the wedge(welding) and the frame.

mmartin

I enclose MC liml file.

MANUEL

JRP

Thanks for the info mmartin, but with such details my calculations will get too complicated. I agree that this is possible with one flange and a tube. But if you want to design a machine, this is too much work and also too much unknowns...

mmartin

You are absolutely right.
MANUEL

disla

HI JRP,

I don't think any structural software include the welding details on the FEM model.

They just extract the forces and moments to be further introduced in the connection model.

They have a huge connection library waiting for the forces and moments to be applied.

You can also do it . Build yourself a library with the typical connections you use and insert the forces and moments computed from your regular structural software.

If you don't want too much detail as Manuel is providing you can still go to simple models made by shells on ccx (they automatically expand to solids)
Merge the nodes where the welds are located (that means conformal meshes which is not always easy to obtain).

There are some references where deviations are estimated depending on the simplification you are doing based on the HotSpot Method.

https://www.apolloedge.com/modeling-welds-for-finite-element-analysis-fea/

The more precise you want the analysis the more you need to work to build a better weld representation.

See if the attached example helps. Ccx is required. Based on the webpage , this is a
Simulation 2.

(Two bodies. No modeled welds. Single bonded contact.) Around a 14% deviation is foreseen.

Regards

JRP

disla thanks for your comments.

First, it is not my intention to model and mesh welds in FEM software, because it is just too much work and I'm too lazy. Maybe just for one particular detail, which needs study in very fine details.

I always make conformal meshes with shell elements. I never use bonded contacts to "glue" plates together in analysis.

I will try CCX solver and then stress linearization. It is just very unpractical because some elements and loads are possible in Internal solver and not in CCX solver. I do a lot of combined element analysis, for example when I want to transfer load to a hole in a plate modeled from shell elements, I usually use link elements.

I will adapt and try with CCX solver and with simplifed analysis with elements and loads that are possible and then report back. I have some work before this...

JRP

I made a quick test with a simple plate 10 mm thickness welded to flange thickness 20 mm. I've attached my test file.
I saw that Stress linearization tool is not what I need, because it is a different kind of tool.

I need simple presentation of stresses in element coordinates UU, VV, UV and in-plane principal stresses 1 and 2 over preselected path.
This is how it is done in Ansys:

https://sites.ualberta.ca/~wmoussa/AnsysTutorial/PP/AdvancedX-SecResults/AdvancedX-SecResults.html

I see some possibility with table result and then export to csv file. After that I could plot a graph using Excel or Python.
There is just one thing I can't set. Is it possible to select a node set. Let's say that I would like to select only 11 nodes where plates are connected and that represents my weld. For that nodes I will select stresses UU, VV, UV, 1 and 2.

JRP

I forgot to mention, that it would also be great if one could select just one set of elements before selecting a set of nodes. In my case that would be selection of 10 mm plate elements and then stresses UU, VV, UV, 1 and 2 for 11 nodes, where the plate is connected to the flange.

disla

Hi JRP ,

I'm glad to see you found a workaround.

You just need to give a name to the set of nodes. In your case you named them Weld 1, so it directly appears when creating a new table in the solution tree. See image.

The only drawback is that nodes appears by defoult in order from smaller to bigger so it is not really a path as it do not reflect the real profile along the weld. For that you need to include the node coordinates and properly order them to match the run.

At the apolloedge webpage they suggest to “add a split line offset from the weld edge. This split line will define the area from which to pull forces and moments.

Offsetting from the edge ensures that the nodes are inside the weld and not shared by multiple bodies.”

JRP

Disla, that is interesting. I created that named node set just because I thought they will appear in tables creation tool. But for me they don't. Check image. What could the reason be?

When this is solved, then is no problem to export node set with all the data to csv file and then make some automation in Python so I get weld report for all welds (node sets I created in Mecway).

Nodes can be arranged according to coordinates with some work. It is only a problem if node set is not oriented parralel with coordinate system axes. But that can aslo be solved with some matehematic work probably and then automated, so nodes are arranged by proper coordinate location, not by number.

disla

It happend also to me. I had to solve again once the table is created for the set to appear.
I'm using mecway 13.1 and ccx 2.17.
Regarding selecting nodes shared by two perpendicular shell elements, i'm not sure what uu, vv and uv means. Thats probably why an small offset is suggested.

disla

You can also reorient the U and V local axis for the elements of interest before solving. This is done in element Mesh --> element properties. This way you can save some post processing and math.

JRP

Disla, yes I folowed your advice and I can add node set to table solution now. Thanks.

I also added two node sets now. One is shared with two plates and stresses are not very logical. If you check UU stresses, I got different results on top node (0 mm, 50 mm, 0 mm) on bottom, middle and top layer of shell elements, which is not logical.
If I move one node into plate (x = 2,5 mm) as you suggested, I get same stresses on all layers. This is just one quick simple check.
It is also good to quickly compare top node from the set (0, 50, 0) and bottom node (0, -50, 0) and (2,5, 50, 0) and (2,5, -50, 0).

I still have to test few things, because this offset will be hard to put into practice, because there is not always a set of nodes in line one node away from plate shared nodes.
But I don't understand what you meant with your last post of reorientation of element axes?

disla

Hi ,

UU and VV would have more sense for me if they are parallel and perpendicular to the weld.
This way they will provide information about the evolution of the Normal and Shear Stress along the weld. If you are using triangles for example or you want to be freer in the mesh shape you want to be sure that all the elements in the plate have the same internal axis orientation. It sometimes happens that when refining some of the elements change orientation. Or maybe just for consistency and easy interpretation of results you want to keep V axis parallel to the weld.

Well, this can be done selecting the set of elements ---> Mesh Tools menu---> Element properties and addressing the direction of the internal U axis.

Check the images too see the difference.

JRP

I understand what you are trying to say, but I never refine my meshes after I mesh and prepare the model. Usually I know from experience what kind of element size will be enough for the good enough results. Now, don't take this test model too seriously, I'm just trying to make a tool which could be used in weld dimensioning.

In this test model I already have U axis prependicular to the weld and V axis parallel to the weld.

I will try one more thing and post it here for some debate...

JRP

I tried it quickly. I made two plate with butt weld. Stress VV in the common node set is exactly the middle value of sets that are located one element in thicker or thiner plate.
There is some averaging going on with common node sets, which is not good.

Victor

Yes, the node values for UU, VV, etc. stresses are simply averaged from adjacent elements so they're meaningless at the join where U and V directions aren't uniquely defined. You should use element values instead (select Element values in the Table options) if possible, otherwise the nodes slightly offset from the joint.

Named selections (and everything else) defined in the modeler are only transferred to the solution and made available to the table during solving so unfortunately, you have do define them in advance.

JRP

Ok. That is good. I thought before to go with elements, but when I select node set and then select element values in table, it also gives me elements for second material, because they belong to that nodes.
I did a test and export everything to csv and then manualy deleted values for 20 mm plate, becaue I'm only interested in 10 mm plate values. This gives me values I need (same for top, middle and bottom which is checked for this test case).
I then arranged nodes according to Y coordinate values and then displayed them in a graph. This is my final result and what I need.

Questions for Victor:
1) Would it be possible to select node set in table selection and then also select one material so that output will only be for that material? It would be great, beacause I had one less operation to delete values I don't need from csv file.
2) How hard would it be to do and code something similar in Mecway as Stress linearization tool, just for the purpose I need? To be able to select preset node set, material and then get a graphical output of values selected. Something similar I did in Excel. Check attached files.

Victor

1) You can do that using a face selection instead of a node selection. It's tricky to select the faces at the connection so what I did was select Plate's elements, use Mesh tools -> Disconnect elements, hide Flange, then select the now exposed faces on the edge of Plate and make a face selection with them. After solving, use that face selection for the table and it includes only the elements that those faces belong to.

2) Not sure. I'll have to look into that later if/when I work on this weld stress feature. Thanks for the spreadsheet example.

JRP

Ok. Thanks. This could also work. But if I will make a Python script, it will probably be easier to filter through correct material in that script, beacuse disconnecting elements and selecting faces and then merging nodes back also takes quite some work.
We have to keep in mind that this example is just for test purpouse. On final models I could have a lot of this plots and when the model is finished I don't like to edit it anymore.