I really like this software. It provides quite friendly user interface and precise results by calculix solver. I am wondering that, is it possible for the user to add point mass to the model for eigen frequency solving. I am not sure if the solver can support the mass point element type.
Thanks again to the software author and tester.
I moved this to Feature Requests category.
Yes, CalculiX supports point masses in form of one-node mass elements (MASS) but they are not yet available in PrePoMax.
Would it be enough to add mass to reference points only? That would be very easy to do since the form for entering reference point data already exists. Only one line with the mass of the reference point should be added.
Yes, I think that it would be sufficient in most cases.
Thanks for your reply. Got it~
Hi all,
is there a way to add a mass to a reference point using the key word editor? If not, what would be a recommended workaround? Mesh a small volume and assign a density to achieve the desired mass and then connect that volume to the structure using rigid body?
Some advice would be very much appreciated!
This should work:
*ELEMENT, TYPE=MASS, ELSET=elset_name
mass_element_number, ref_node_number
*MASS, ELSET=elset_name
mass_value
Thank you for the advice. I will give it a try an report.
Hello all,
i tested the keyword definition. That seems to work fine.
All I had to do was to replace the numer of the new mass element with one that was not allready occupied and to add an additional keyword to apply the gravity load to the newly created element.
Thank you for your help!
I see one problem now. The gravity load must also be applied to the mass elements. Now the user selects the domain for the gravity load using the mouse selection. But reference points (where the mass would be) cannot be selected using the mouse. So no gravity will be applied to the mass elements. Currently, a new gravity load must be created for each reference point. That will be confusing for the user.
I think the gravity load (and centrifugal load) should, by default, include the entire model.
Indeed, that can be a serious issue. Maybe the addition of point mass elements should be postponed until reference point selection is implemented in the future.
In Abaqus, the whole model is selected by default (can be changed to a specific region) for gravity load but not for centrifugal/rotary acceleration force or general body force defined as force per unit volume.
I agree, that gravity should by default be applied to the entire model!
Hi all,
I ran into another issue with defining an Element Type=Mass in the keyword editor. In fact, that problem seems to be independend from the type of element that is created using the key word editor (I tried Type=Mass and Type=T3D2 [Truss]) element.
As soon as i use the option “composite” on the shell card:
I get the error message in the screenshot below.
When I deactivate the composite on the shell card:
the model solves as before:
The failiure of the Type=Mass element definition is idenpendend of the shell element type, that must be changed to S8R for composite definition.
I get the same issue with truss element.
Does anyone know a reason, why it does not seem to be possible to combine element definition in keyword editor with “composite” option on shell card?
Many thanks in advance for any advice!
Can you share the file for which this error occurs ?
Yes, file is attached below.
Composite Option with manual Element definition.pmx (3.5 MB)
This is indeed strange. It might be a good idea to report this issue on the CalculiX forum and share the input file there.
I found a realted post in the calculix forum.
Layered shell (composite) with spring element - CalculiX
Apparently, this issue can be fixed somehow by changing the file changekon.f (see last post). I assume this is a file within calculix somewhere, but i do not know how/if i can try editing the file within PreProMax context. Is that at all possible or would it only work if I use Calculix without PrePoMax?
Strange side note: if I deactivate all but one layers of the composite shell, there is no error anymore. Does help in understandig the issue in any way?
Yes, you would have to edit CalculiX’s source code: Search · changekon.f · GitHub and recompile the solver.
For now, we can revive that thread on the CalculiX forum and report this issue here hoping that Guido will take a look at it eventually: Issues · Dhondtguido/CalculiX · GitHub
Ok, thank you. Editing sourcecode is not really within my grasp.
and tried to revive the tread here:
Layered shell (composite) with spring element - CalculiX
I just noticed a similar issue with *DISTRIBUTING COUPLING using *ELEMENT,TYPE=DCOUP3D.
The model does not solve as soon as I define more than one layer in the shell section (with only one layer defined, it works). But this time I do not get an error message, just the information “Job failed - no results exist.”
Composite Option with ELEMENT,TYPE=DCOUP3D.inp (914.1 KB)
This subject is moving away a bit from the original topic. Should we move it to a new thread?
