Problem with creating surface by 'comp' command in CGX

CalculiX GraphiX
1

Hi there,

My intention was going to apply a 3D bolt pretension by a surface and a node. I partitioned a cylinder by a plane in Salome and made a face group of the interface ‘pret’ and a bottom face of cylinder ‘bot’. Then I exported the mesh as unv file and coverted to inp file.

In cgx, I used ‘comp nodeset do’ and ‘send nodeset abq surf’ to export surfaces. I succeeded with the ‘bot’ surface, as shown below, however, in pret.surf file, the element faces was empty. I don’t know why, probably due to partition? How could I create such a surface for bolt pretension? Thanks in advance.

image
image636×257 22.6 KB

Best regards,
William

2

Hello,
maybe you can post what is in your set pret,
if you ask with prnt se !?
than we can have a look ?
maybe there is something missing in your set ?
wbr

3

Hi Dichtstoff,

Thanks for your reply.

I can see from cgx help document for command send that it probably doesn’t work for such an internal face due to partition operation. But then could it be possible by other command/approach if I am going to generate such a surface to apply pretension card?

send top abq sur
will write the elements in set top together with the face-nr (Important: Only
free surfaces of the mesh are regarded, internal faces are unknown and can not
be identified).

I attached my prnt se for your information.

internal_face
internal_face1193×623 65.3 KB

BR, William

4

Hello ,

i don’t see no reason why it should not work with both sets.
but for better understand i recommend you always to have a look
on your sets after each command!
where you get the (surf)faces? from the elements in your set !?
you have to fill your set with elements (from nodes) and from elements you
get the (surf)faces !?. Maybe you have to use the commands often (twice)
or you have to use comp set up !?
you have to play a little bit and check always
with prnt se and plot f bot

wbr

wbr

5

Hello William,
you identified the problem correctly. Unfortunately cgx does not create internal element faces and can not deal with them. I see only the possibility to create a set of the relevant elements. Then write this elements with the send command to the filesystem (send set frd c)and open this file again in a second cgx session. There you create a set of the now visible faces (qadd set t1) and export them in the usual way.

Best regards,
Klaus

1 Like
6

Thank you very much Klaus, finally I got succeeded according to your suggestion.

hcpy_1
hcpy_1784×656 30.8 KB

7

In my analyzes, I divide the bolt into two parts A and B, then:

  1. create a mesh from part “A” ,
  2. send the surface,
  3. create a mesh from part “B”,
  4. and finally connect both meshes.

mesh S_A
COMP pre do
COMP pre do
SEND pre abq sur
mesh S_B
merg n Bolt
send abq Bolt

pre

2 Likes
8

Hello Klaus and William,

Thank you very much for your replies on this topic. They helped me solve the problem of defining the pre-tension surface for my simulation.

I did the same, but made a small change to automate the process using the ‘enq’ command.

For example, in a main.fbd file:

Reads the mesh and selects the elements from the node set. After that, deletes the mesh.

read Mesh.inp
comp Elements_from_node_set up
send Elements_from_node_set frd c
del mesh

Reads the element set and selects the faces from the elements set to create the surface.

read Elements_from_node_set.frd
comp all up
enq all Surface_from_nodes rec _ _ 0.1
comp Surface_from_nodes do
send Surface_from_nodes abq sur

After that, I can import the Surface_from_nodes.sur in my solve.inp file

9

@Tombs42 thank you for your note which brought this thread onto surface.

In modeling a pretension, how are the top and pret surfaces related to one another? Is it applied as a relative deformation between the two?

10

Hi @fethio,

I’m glad to be able to maybe contribute. From the documentation, I understand that there are two ways. But, as you mentioned, they are all a relative displacement between the split surfaces.

The first is to apply a constant force using Cload to the node using PRE-TENSION. For example:

Let’s say that the top is SSurface_from_nodes.

*PRE-TENSION SECTION, SURFACE=SSurface_from_nodes, NODE=Ref_Node
0., 0., -1.
…
*Cload
Ref_Node, 1, 490000.0

Secondly, apply a displacement with a fixed Boundary, using the previous step with op=MOD.

*PRE-TENSION SECTION, SURFACE=SSurface_from_nodes, NODE=Ref_Node
0., 0., -1.
…
*Boundary, op=MOD
*Boundary
Ref_Node, 3, 3, 0

I have used both. First, in the second step of my analysis, I applied force and displacement to simulate other loads applied to the structure. However, I’m still working on it to achieve better results.

This example was the best for me: Bolted Connections - #5 by JuanP74

Please let me know if this answers your question, and we can discuss finding a better solution.

11

Thank you @Tombs42 . I got confused a little. You mentioned that there are two ways (I did not check the documentation yet, but I have also concluded there are even more than two ways to include a pretension with, 1) using the initial stress card, 2) applying relative displacement in a magical way, 3) by changing temperatures, etc.

It seems the initial stress card is not able to produce accurate results, especially at around the gasket joint, which is mentioned as crucial by @Disla

In your post, you mention The first ... and then Secondly ... I was not able to figure out whether these two corresponded to STEPs in a single analysis, or they were alternative ways to get the pretension. Is there interpenetration as a result of applied relative displacement at the plane dividing the shank into two parts?

I have an interesting eigenvalue problem that I would like to test the bolt pretension, with the aim to model the piezo disc assembly in an ultrasonic transducer.

12

Hello @fethio

Sorry for the confusing, I will try to learn more and explain better what I tried to do in my recent analysis of bolted joints. I’m quite new here and in using CalculiX as a FEA tool.

You are right. What I mean by the two ways is by only using the *PRE-TENSION SECTION. But certainly other options can be used with CalculiX for simulating bolted joints as you mentioned. They can also be used together.

In this option, " The parameter NODE is used to define a reference node. This node should not be used elsewhere in the model. In particular, it should not belong to any element. The coordinates of this node are immaterial. The first degree of freedom of this node is used to define a pre-tension force with *CLOAD or a differential displacement with *BOUNDARY."

What I`ve been trying in my analysis is using first the pre-tension force in a first step, and after that setting the differential displacement as the boundary in the next step. Maybe, I can use directly a displacement, not sure yet. What do you think? Maybe I can share it in another topic.

Thank you very much for your attention! Later, I will share here an example.

13

@Tombs42 if you are intending to open a new topic about this, you may consider inquiring about the *INITIAL CONDITIONS card (ccx/node304.html) as well as the *PRE-TENSION SECTION card (ccx/node334.html). It may be worthwhile to learn about the possibility of the use of the former card to define pre-stress in an element group.