INIVEL units and CArbon Fiber Modeling with Mixed Approach
Hello,
maybe thats a dumb question but I want ti ask about the units in INIVEL. I set the unit system in the begin card to mm/s/kg.
Is it then for the velocity mm/s?
I ask this because in the manual it says its either m/s or rad/s. Also the part gets destroyed a lot when I set INIVEL for a crash to 4000, which I really dont expect in a crash with around 14kmph.. Or maybe my model is the problem.
Answers
-
Hi Zeynep,
The model set up should be done based on the units you have set in the /BEGIN_CARD. In RADIOSS help (or manual) you can see the units proposed for its value given as an example (most of the times in S.I. units). So, if you see m/s it means (length unit)/(time unit) and then you have to adjust it in the unit system that you set in /BEGIN Card. Overall, you are correct, your values should be in mm/s!
The /INIVEL load can be used for both translational and rotational movement, so this selection has to modify the units used. The selection between the two types can be done through the 'type' variable. So, accordingly to that units are modify as m/s or rad/s and adjust to the system you have set in /BEGIN Card too.
Finally, the value 4000 you are using it should be the problem. I personally have run some models with higher values than this and the same unit system. What exactly do you mean when you say the model destroy? Feel free to share more info of your model to clarify what is going wrong!
Polyvios
0 -
Heyy, thank you for your help. It is a crash simualtion of a passenger cell that is out of carbon fiber on a rigid wall. I used differnet values for the speed but it gets completely destoyed in the front as I said even for 10kmph. I think I might have made mistakes with modeling the materials. I used different approaches for modeling carbon fiber, PCOMPP, P51Stack, P11 etcc. My MAterial is MAT25 for both Honeycomb and Carbon Fiber. some mechanical values that I know I put in the material card, for the rest I found some card examples from Altair etc
Zeynep
0 -
Zeynep Aydin_22555 said:
Heyy, thank you for your help. It is a crash simualtion of a passenger cell that is out of carbon fiber on a rigid wall. I used differnet values for the speed but it gets completely destoyed in the front as I said even for 10kmph. I think I might have made mistakes with modeling the materials. I used different approaches for modeling carbon fiber, PCOMPP, P51Stack, P11 etcc. My MAterial is MAT25 for both Honeycomb and Carbon Fiber. some mechanical values that I know I put in the material card, for the rest I found some card examples from Altair etc
Zeynep
Hi Zeynep,
Is it possible to share any photos showing the destroyed front? It will be really helpful to understand the problem!
Polyvios
0 -
Polyvios Romanidis said:
Hi Zeynep,
Is it possible to share any photos showing the destroyed front? It will be really helpful to understand the problem!
Polyvios
Hi Polyvios,
first of all I want to thank you again for all your answers to my questions.
I added the model in the attachments. But in this version I modeled it know with the mixed approach. Before that I used shell elements also for the honeycomb and didnt model the materials correctly. In this version as I said in another question, I have problems with the contact definition. I am not sure how to combine the nodes for the parts. I guess I have to change the mesh completely. In another version (Front_Impact_36kmph_M46J_T800S_PCOMPP_Mixed_Model) I modeled it the way, that I have a gap of 0.8mm between the shell and the core. With that I had less penetration problems. But this way the modell is alos not modelled correctly I think, because I forgot to apply INIVEL to the inner layer and of course it didnt move. So with this way I guess its not modelled correctly because the layers are glued to the honeycomb in reality.
Now I dont really know what is the best way and how I can get more accurate results.
I am sorry that I mixed the topics and put everything in one thread now.
Best regards
Zeynep
0 -
Zeynep Aydin_22555 said:
Hi Polyvios,
first of all I want to thank you again for all your answers to my questions.
I added the model in the attachments. But in this version I modeled it know with the mixed approach. Before that I used shell elements also for the honeycomb and didnt model the materials correctly. In this version as I said in another question, I have problems with the contact definition. I am not sure how to combine the nodes for the parts. I guess I have to change the mesh completely. In another version (Front_Impact_36kmph_M46J_T800S_PCOMPP_Mixed_Model) I modeled it the way, that I have a gap of 0.8mm between the shell and the core. With that I had less penetration problems. But this way the modell is alos not modelled correctly I think, because I forgot to apply INIVEL to the inner layer and of course it didnt move. So with this way I guess its not modelled correctly because the layers are glued to the honeycomb in reality.
Now I dont really know what is the best way and how I can get more accurate results.
I am sorry that I mixed the topics and put everything in one thread now.
Best regards
Zeynep
Hi Zeynep,
Thank you for adding all the issues you want to discuss in one case in order to handle this better!
I cannot think of a way to model honeycomb materials with 2D elements in a 3D model. Instead you should use the /MAT/LAW28 and solid elements (also PROP_TYPE6).
If you want to create a mesh with coincident nodes between solid and shell elements, the best way to achieve it is by first creating the shell elements and then use the HEX module in 3D mesh ribbon to create the solid elements between the shell elements surfaces. Using this tool you can set the shell elements of the first surface as source elements and the shell elements of the other surface as target elements. The final model should have neighbor solid and shell elements sharing the same nodes.
In Picture 1 you can see a shell-solid-shell mesh layout. If you want to try the results of this technique, try to move one of your elements and see if its neighbor deforms by this movement.
If you want to model the shell-solid connection with an interface, TYPE7 interface is not recommended. Instead you should use a TYPE2 interface which acts like a kinematic condition. TYPE7 is for modeling contacts but if your bodies are not going to touch, for example if they move parallel to the plane of their interface, you wont see any interaction between them. In contrast, TYPE2 interface will make the bodies move together in any movement that occurs.
Regards,
Polyvios
0