I am reading the Calculix Input code guide and would like to understand more about how the .inp file is written. Here are some quaestions I have about it. I did a 2D plane stress test:
What is the meaning on the heading of: Hash: Qr6Q0FwL How is this written?
How is the name of the Aditional sets is generated? I created 2 ref. points. How is there name selected/gven? (ref_170561/ref_170562/ref_170581/ref_170582)
Thse 2 Nset and Eset generate when I select 2 contact pair surfaces, thus I imagine that both refer to the same surface one being the sets of nodes and the other being the set of elements in that surface??
When defining the constraints, why do I need to have 2 nodes placed in the same position with different index (17057 and 17058 are in (0,0) position), to say the reference node and the rotation node? These generated extra Nsets, and makes extrange things in the BC definitions also…
may I just erase the Rot node??
Apparently, it’s generated by GetRandomString(8) function. Of course, you don’t have to include it in your input files, the whole *HEADING is optional.
It’s just the last mesh node number + 1 for REF NODE and +1 again for ROT NODE. Then it continues with increments of 1 for further reference points.
Yes, those are internal node and element sets generated for your manual selection. Abaqus also converts so-called geometrical sets to node/elements sets when writing an input file.
Yes, those are the labels including numbers of element faces. Check the *SURFACE keyword in the CalculiX manual.
That’s just what CalculiX’s syntax for *RIGID BODY requires:
For the rotational degrees of freedom a dummy rotational node is used whose translational degrees of freedom are interpreted as the rotations about the reference node. Thus, the first degree of freedom is used as the rotation about the x-axis of the rigid body, the second as the the rotation about the y-axis and the third as the rotation about the z-axis. The rotational node can be defined explicitly using the parameter ROT NODE. In that case, this node must be been assigned coordinates (their value is irrelevant) and should not belong to any element of the structure. In the absence of any of the parameters REF NODE or ROT NODE, extra nodes are generated internally assuming their tasks. The position of the default REF NODE is the origin.
Thank you very much for your pront response @FEAnalyst . Just a couple of doubts athat arise from your answers:
I do not understand. Because in that case the 2nd ref point Nset should be 170563 and not 170581. Moreover when you say the last mesh node number … I have 31017 nodes in my model so I do not know where these 170561 and 170581 come from…
I checked the maual as you suggested, but do not understand how is the numbering ,which is the logic or how do I know which is the right number to put?
In my case this is the mesh I have and type of analysis, however how do I know which of the 3 options is the right one? how can I know which surface of the element correponds to each number?
Maybe you have some additional nodes from other features. Just check the *NODE section of the input file (in keyword editor or after exporting). You should have your mesh nodes and then at the end the two nodes for REF NODE and ROT NODE. Like the last two here with coordinates (1,2,3) to find them easily:
It’s based on node numbering. But it’s usually handled by preprocessors as it would be hard to do it manually for 3D elements. You would have to identify the node numbers for a given face, check the definition of the element and compare with numbering in the documentation. I recently explained it here: Export .inp mesh with node sets - Page 2 - FreeCAD Forum
Which version of PrePoMax are you using ? The input file importer is outdated by it works for me in 2.1.0 and 2.1.10. You may just have to redefine some features that were not recognized properly by the importer.
But since you have the whole input deck, why don’t you submit it using standalone CalculiX outside of PrePoMax ? You will just have to correct this:
*ERROR in splitline: there should not
be more than 16 entries in a
line;
1,2,3,4,5,6,7,8,9,10,11,12,13,14,15,16,17,18,19,20,
I was using version downloaded: 11th of september. I rechecked and downloaded the one from 13th of september now. SO will try with that one as soon as I can.
I corercted the fact that I had 20 entries. But appeared 1 new error and thousands of warnings.
I am worried about the one of surface behaviour. Why is this warning appearing?
SInce I have so many warning I cannot see where the error is coming from.
Did you correct all the node/element set definitions ? There’s a maximum number of 16 entries per data line. If you scroll up in the command window, you may see more *ERROR messages.
I wrote outputfile.txt, a .txt file should be generated when runned? or which is the extension of the file i should check to know about the error informatio?
Yes, but you should run the entire command and add a symbol > at the end with the output file name. You can choose any extension. The file can later be opened in a txt editor.
Is it posible that the node numberng order is different in calculix than in other programs?
A counterclokwise numbering of nodes in a quadrilateral element should give a positive normal, right?
The problm is that I tried numbering them counterclokise and clockwise and gives the same error in both…
The positive normal is given by the right-hand rule going around the nodes in the order in which they appear in the element definition. So yes, it should be counterclockwise for 2D elements. From what I checked before, the bottom part (rack) had it opposite in the file you shared. The top one (gear) was ok.
This time it’s a different issue - node adjustment in contact. Just remove the Adjust parameter and it will work. It may fail to converge but that’s another issue - try without the applied moment (use only small rotation of the rack reference point) and fix the rotation of the gear for now. Contact definition may also need some corrections.
