Is it possible to read CFN and CFS values at intervals of L/4 along a fillet weld, which is defined within a single tied contact in a surface-to-surface interaction model? Or would it be necessary to create separate contact surfaces and tied contacts at intervals of L/4 along the weld to read CFN and CFS values individually?
Yes, you should create multiple contact definitions to read the total forces from selected patches…
Besides using multiple contact definitions, are there alternative methods to extract force values from contact elements? Does anyone have knowledge or experience in this area
You don’t need additional contacts. Forces and Moments can be extracted with *SECTION PRINT.
I guess the only difficult part is how to access those internal faces. I’m using Mecway. Not sure how it works in other software.
Are you talking about contact forces (on contact surfaces) or internal forces (not on free surfaces in contact) ?
Section print gives total forces per surface so it would have to be defined for each patch, right ? Also:
Since the section forces are obtained by integration of the stresses at the integration points of the faces, which are obtained by interpolation from the stress values at the facial nodes (which in turn are determined through extrapolation from the integration point values inside the volumetric elements and subsequent averaging over the elements to which the node belongs) they will not be accurate at locations where the stress jumps, such as at interfaces between different materials.
Surface in general. Not only free or contact surface. Give it a try.
Regarding that note on the manual I read it as usual:
Stress interpolation could be inaccurate at locations where the stress jumps. It is not exclusive of section forces.
I know but I was wondering why you mention (and show in the screenshot) internal faces and difficulties with their selection.
Maybe I read wrong your comment.
I mean that there is no need to define a contact or split the body to extract forces on a section inside the body. One can extract them as far as you can select them. That is the tricky part.
My bolt in the image is a full body without any contact and I’m extracting the section forces.
1 Like
I’m a bit confused. My goal is to define a single contact on the surface we’ve identified, but to extract Fshear and Fnormal regionally across the entire surface. As you can see in the image below, I’ve manually divided the surface of each part to extract contact forces. However, when I want to define numerous parts, it takes too much preprocessing time. I believe there are scripts in ANSYS to extract forces via contact elements, and I assume there must be similar capabilities in CalculiX. Unfortunately, I’m unsure of how to proceed. Any guidance would be appreciated
Ok, I see. I assume that the OP needs contact anyway but maybe it’s not necessarily the case.
@osmcnkrtn Surface partitions could be less time-consuming. You can do them even in FreeCAD.
If you check the table with output variables in CalculiX manual, you will see that there’s not much to choose from. You can write the number of contact elements but not their individual forces. Only total forces are computed.
1 Like
The idea is that you can request SOF and SOM of any surface. What one typically does is to select free surfaces (at the envelope of the body) or contact surfaces.
But there are other surfaces. The FE discretization is made of pieces like a LEGO (elements) and they also have faces each one although some of them are not directly selectable.
If you find the way to expose those faces , you will be able to request SOF and SOM of those faces.
Mecway has some tools to do that as it allows to hide certain elements and expose those hidden faces.
If you could hide some elements by color in your model, those sections could be exposed.?¿? Jakub has a good knowledge of Prepomax. Maybe he can find a workaround. The problem I think could be that Prepomax erase all those faces that are not used.
1 Like
Currently, it’s not possible to hide individual elements in PrePoMax so there are two ways:
- partitioned volumes (already used by the OP)
- creating element sets and converting them to parts so that they can be hidden - not very convenient but often helps
1 Like
I’m actually confused about one point: when I define a single surface contact, I can output CFN and CFS as resultant forces. However, in reality, the code is performing element-wise summation in the background and then shows the total sum of the results(as i know). It should be writing the element-wise contact force values somewhere. Do you think it’s possible to write these element-wise contact force values to a .txt file? What I actually want is the step just before the CFN and CFS post-processing
CalculiX is open-source. You would have to take a look at the source code and try to figure it out but it may not be so easy. For now, you can create a feature request here: Issues · Dhondtguido/CalculiX · GitHub
Abaqus has the CFORCE output variable (consisting of CNORMF and CSHEARF), making it possible to create contour plots of contact forces.
CalculiX has CSTR (contact stress) field output but you would need a corresponding area to integrate it to get forces.
1 Like