Stuck? 
support@mecway.com
support@mecway.com
Mecway
FEA
Stress output for weld calculation
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?
I know this is not possible in Mecway, but maybe there is some other way to get to something useful?
Howdy, Stranger!
It looks like you're new here. If you want to get involved, click one of these buttons!
Comments
¿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.
I have most of the models built from shell elements. I'm looking for something like that.
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
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.
MANUEL
MANUEL
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
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...
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.
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.”
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.
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.
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?
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.
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...
There is some averaging going on with common node sets, which is not good.
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.
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.
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.
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.