1D Beam (CBEAM) End Offsets Question
Hello,
I have a cylindrical shell which is stiffened longitudinally using beams. I want to represent the stiffeners using 1D Beam elements. And I have created a custom Cylindrical Coordinate System. I want to offset the node ends (B & A) in the radial direction. I am unable to find a way to achieve the same. The only option I know how to perform offsets is using Bars > Update panel and in that panel, I don't see an option of selecting the desired CSYS.
Please help...
Thanks.
Answers
-
Altair Forum User said:
Hello,
I have a cylindrical shell which is stiffened longitudinally using beams. I want to represent the stiffeners using 1D Beam elements. And I have created a custom Cylindrical Coordinate System. I want to offset the node ends (B & A) in the radial direction. I am unable to find a way to achieve the same. The only option I know how to perform offsets is using Bars > Update panel and in that panel, I don't see an option of selecting the desired CSYS.
Please help...
Thanks.
Hi,
In panel 1D>bar has switch 'offset in displacement' means the offset values are based on Displacement System of grid (nodes), so you just need to assign nodes of cbeam to your cyl system,
enter panel analysis>system>assign select nodes of cbeam, your cyl system and 'set displacement'
0 -
Thanks Sir for the reply. I will try out your suggestion.
0 -
Hi,
I have a follow up question regarding the above. I am now facing issue with beam orientation. I have several stiffeners around the circumference and I was able to get the beam C/S oriented correctly by defining a vector (radially). However, when I use that vector for defining the beam orientation for other elements, I am getting inaccurate output. I wish to use the custom cylindrical CSYS I have created to define the beam element orientation as well but I am not able to get it to work in Hypermesh. I even tried Analysis->System->Assign->Set reference feature but it didn't seem like it did much!
I would appreciate help in setting up beam orientation using custom cylindrical CSYS in Hypermesh.
Thx
0 -
please find attached video for same.
0 -
Hello Rahul,
Thanks for posting the video. It was helpful. But my issue is a little different. Perhaps a couple of pictures to illustrate may help.
I am representing the stiffeners using 1D Beam elements. Currently, I am experiencing issues with orientating the Beam C/S. In other Nastran based FE pre-processors, I can orient Y-Axis of Beam C/S using the custom CSYS.
0 -
0
-
Hi Tinh,
Thanks for the reply. That is exactly I am looking for. Unfortunately, my copy of Hypermesh is not importing or displaying contents after importing bdf files. I tried importing other bdf files as well and I am having no success. I probably need to contact Altair Customer Service to figure out the issue.
In the mean while, I am wondering if it would be possible for you to post screenshots or instructions on how you achieved correct beam orientation in the above model?
Thx
0 -
Altair Forum User said:
Hi Tinh,
Thanks for the reply. That is exactly I am looking for. Unfortunately, my copy of Hypermesh is not importing or displaying contents after importing bdf files. I tried importing other bdf files as well and I am having no success. I probably need to contact Altair Customer Service to figure out the issue.
In the mean while, I am wondering if it would be possible for you to post screenshots or instructions on how you achieved correct beam orientation in the above model?
Thx
If you have trouble with beam section orientation, switch orienttation to 'node' and supply G0 as a node on axle of the tube, then you can specify offset ay, by in 'element coord system'
0 -
Thanks Tinh,
Your suggestion totally worked.
I hope this issue will be the final one from my side. Is there any way to reverse element direction in Hypermesh? I am seeing that some of my 1D elements have their Z directions in wrong direction and hence the base leg of my L-Angle are oriented in opposite directions. I couldn't find an option to reverse or modify element co-ordinate system.
0 -
you can modify it by update beam orientation (y axis), but x axis is always nodeA--nodeB
0 -
Tinh,
Thanks again for replying. Actually, I wanted to modify the Z direction of my beam element. Can you help me out on how to do that in Hypermesh?
0 -
Altair Forum User said:
Tinh,
Thanks again for replying. Actually, I wanted to modify the Z direction of my beam element. Can you help me out on how to do that in Hypermesh?
Hi , if you modify orientation (y axis) then z direction is modified, too.
0 -
Tinh,
As you can see, the Y axis are oriented in the direction I want, but it is Z (and also X) that I want reversed. Is there a way to reverse element directions in Hypermesh?
Thx for your support so far.
0 -
Hi
It is due to direction from nodeA - nodeB of your beams was changed
I think you should re-create the beams
Do you use '1D>line mesh' panel?
create a temp comp named ^temp
enter 1D>line mesh , switch 'lines' to 'node list' => 'node path'
select nodes from one end to remain
switch elem type to 'bar'
select orientation same as one of correct original beams
->mesh
-> delete original beams and move new beams from ^temp to original comps
0 -
Thanks again for your reply. I will try your suggestion. But I have to say that the above sounds a little tedious. I don't understand why Altrair did not provide a simple element reverse option.
0 -
Altair Forum User said:
Thanks again for your reply. I will try your suggestion. But I have to say that the above sounds a little tedious. I don't understand why Altrair did not provide a simple element reverse option.
I think so. if you usually face the problem, I can write a tcl script to reverse it. Many functions Altairian think rarely used, so they didn't provide it
0 -
Altair Forum User said:
Thanks again for your reply. I will try your suggestion. But I have to say that the above sounds a little tedious. I don't understand why Altrair did not provide a simple element reverse option.
Please try this way
0
