I am trying to model the process of Automated Fiber Placement. However, I want the model to be more realistic through having a moving roller and multiple layers of tapes.
In Abaqus, I am using STANDARD solver to make use of the MODEL CHANGE feature to deactivate/activate parts.
How can I model the contact between the roller and tapes through the general contact (with cohesive property) as some parts are deactivated until its turn comes.
I believe some of our Abaqus colleagues can help you. @kmao24 @tao364744553 @BoPeng @Haodong
Thanks for your concern. Hope so.
just like the model change from step to step, the general contact can also be updated from step to step. for example, after defining the general contact in the model definition part (before the 1 st step), you want to exclude the surfaces A and B from the general contact in Step-1, you can use
*contact
*contact exclusions
A, B
in Step-1. Then in Step-2, if you want to include surfaces A and B contact in Step-2, you can use similar keywords like
*contact
*contact inclusions
A, B
in Step-2.
many thanks for your response. I tried what you mentioned, but still not working. could you check the this model. 0000
hi, Ahmed,
I looked at your model, and it seems that there are a number of modeling issues, in additioin to the contact change question you mentioned earlier:
1- the cae model says the model does not have the specific heat defined, since the model is using a coupled tmperature-displacement procedure. In this procedure, the transient heat transfer analysis is involved, in which physically the specific heat (a physical property has to be defined.
2- the model uses the elements with temperature degree of freedom for the coupled temperature-displacement simulation. Do you really want to do a coupled heat transfer simulation? If you want to model a structural simulation in which something (like the material property, thermal expansion effect, etc.), you do not have to use a coupled temperature-displacement simulation. If you already know the temperature change, you can apply it to the structure without the need to solve for the temperatures. Solving the temperatures is the task of a coupled simulation. If you know the temperature change beforehand, you can simply apply the temperature change without the need for the coupled thermal-structure simulation.
3- last time, I thought you were using the general contact for the contact change (since you mentioned the general contact). The recent cae file shows you are using the contact pair approach. For either the contact pair or the general contact, you can temperarily deactivate and later re-activate the contact, although the way of their definitions is slightly different.
4- if you are not familar with each feature, I suggest you create a simple model and execise each feature. It will be easy for us to help you with a simple model with a specific issue.
Regards, kmao24
Hi, kmao24
Appreciate your words. I have wrongly sent the wrong model. Correct one is here 0000 .
hi, Ahmed,
Here are my comments after looked at your model:
1- The feature to modify the general contact from step to step is available in abq2023. However, its GUI interface is available after abq2024. It seems you are using abq2023. This may be the reason you are unable to define it in your cae version, and you used the contact pair. In other words, your model uses the mixed general contact and contact pair approaches which could cause confusion in the model. Even without CAE UI in abq2023, you can use the keyword editing to achieve your purposes for the contact change, like I responded to you first time.
2- you can deactivate the intended contact pairs, and you do not need to deactivate the related parts. I saw your model also deactivate the parts like prereg. This is not necessary, and sometimes it can cause numerical issues if it is not done properly.
3- for the upper end of prereg, you use tie in order to use a reference point to control the end. The best way is to use the kinemaric coupling to couple the RP to the end surface of the prereg, just like the coupling between the ring inner surface and the ring center. Also, the prereg end controling point (RP) has to be fixed.
After these treatment, your model is able to run for the first 2 steps. it is still running at time of writing.
Note that I will be out of two for the next 10 days, and unable to check your updates.
Regards, kmao24
Hi Kmao24,
Again, many thanks for your explanation.
1- yes, I am using Abaqus 2023. I am not getting how to activate/deactivate contact pairs in the inp file, could you share a screenshot or the inp file so I can grasp it.
2- I am using activate/deactivate parts because there are many of them and need to be placed in order.
3- I have tried the coupling constraint and it gives error. This is the reason made me go for tie interaction.
I wonder if the model completed the job after your modifications!
Regards, Ahmed
hi, Ahmed,
I try to attach the modified inp file that runs for the 1st 2 steps. However, it does not allow me to do it, since it is not an authorized format. Is that any way to upload a text file?
I put the keywords and definitions below:
** INTERACTIONS
**
** Interaction: General
*Contact
*Contact Inclusions, ALL EXTERIOR
*Contact Property Assignment
, , Normal
Tool , Prepreg-Down , Cohesive
Tool , Prepreg-Down-2 , Cohesive
Tool , Prepreg-Down-3 , Cohesive
Prepreg-Down-3 , Prepreg-Up , Cohesive
Prepreg-Down-3 , Prepreg-Up-2 , Cohesive
*Surface Property Assignment, property=GEOMETRIC CORRECTION
_General_gcs0_3, Circumferential, -2.11636e-16, 0.02, -0.0025, -2.11636e-16, 0.02, 0.9975
_General_gcs0_6, Circumferential, -2.11636e-16, 0.02, -0.0025, -2.11636e-16, 0.02, 0.9975
_General_gcs0_9, Circumferential, -2.11636e-16, 0.02, -0.0025, -2.11636e-16, 0.02, 0.9975
_General_gcs0_11, Circumferential, -2.11636e-16, 0.02, -0.0025, -2.11636e-16, 0.02, 0.9975
_General_gcs0_30, Circumferential, -2.6942e-07, 0.02, -0.0075, -2.6942e-07, 0.02, 0.9925
_General_gcs0_33, Circumferential, -2.6942e-07, 0.02, -0.0075, -2.6942e-07, 0.02, 0.9925
_General_gcs0_36, Circumferential, -2.6942e-07, 0.02, -0.0075, -2.6942e-07, 0.02, 0.9925
_General_gcs0_38, Circumferential, -2.6942e-07, 0.02, -0.0075, -2.6942e-07, 0.02, 0.9925
_General_gcs0_45, Circumferential, -0.0475, 0.02, 0.0349997, -1.0475, 0.02, 0.0349997
_General_gcs0_48, Circumferential, -0.0475, 0.02, 0.0349997, -1.0475, 0.02, 0.0349997
_General_gcs0_51, Circumferential, -0.0475, 0.02, 0.0349997, -1.0475, 0.02, 0.0349997
_General_gcs0_53, Circumferential, -0.0475, 0.02, 0.0349997, -1.0475, 0.02, 0.0349997
_General_gcs0_58, Circumferential, 0., 0.021, -0.0035, 0., 0.021, 0.9965
_General_gcs0_59, Circumferential, 0., 0.021, -0.0035, 0., 0.021, 0.9965
** ----------------------------------------------------------------
**
** STEP: Step-1
**
*Step, name=Step-1, nlgeom=YES, inc=10000
*Coupled Temperature-displacement, creep=none, deltmx=1.
0.1, 0.1, 1e-50, 0.1
**
** BOUNDARY CONDITIONS
**
** Name: BC-RP-1 Type: Symmetry/Antisymmetry/Encastre
*Boundary, op=NEW
Set-RP-1, ENCASTRE
** Name: BC-RP-4 Type: Symmetry/Antisymmetry/Encastre
*Boundary, op=NEW
Set-RP-4, ENCASTRE
** Name: BC-RP-6 Type: Symmetry/Antisymmetry/Encastre
*Boundary, op=NEW
Set-RP-6, ENCASTRE
** Name: Roller_Fix-1 Type: Displacement/Rotation
*Boundary, op=NEW
** Name: Roller_Velocity-1 Type: Velocity/Angular velocity
*Boundary, op=NEW, type=VELOCITY
_PickedSet867, 1, 1
_PickedSet867, 2, 2, -0.01
_PickedSet867, 3, 3
_PickedSet867, 4, 4
_PickedSet867, 5, 5
_PickedSet867, 6, 6
** Name: Tool-Fix Type: Symmetry/Antisymmetry/Encastre
*Boundary, op=NEW
_PickedSet761, ENCASTRE
**
** INTERACTIONS
**
** Interaction: General
*Contact
*Contact Inclusions
Tool , Prepreg-All
Roller , Prepreg-Up
*Contact Exclusions
, Prepreg-All-2
, Prepreg-All-3
**
** OUTPUT REQUESTS
**
*Restart, write, frequency=0
**
** FIELD OUTPUT: F-Output-1
**
*Output, field, frequency=2
*Node Output, variable=PRESELECT
*Element Output, directions=YES, variable=PRESELECT
*Contact Output
CDISP, CSDMG, CSQUADSCRT, CSTRESS
**
** HISTORY OUTPUT: H-Output-1
**
*Output, history, variable=PRESELECT
*End Step
** ----------------------------------------------------------------
**
** STEP: Step-2
**
*Step, name=Step-2, nlgeom=YES, inc=10000
*Coupled Temperature-displacement, creep=none, deltmx=1.
0.001, 2., 1e-50, 2.
**
** BOUNDARY CONDITIONS
**
** Name: Roller_Velocity-1 Type: Velocity/Angular velocity
*Boundary, type=VELOCITY
_PickedSet867, 1, 1, -0.05
_PickedSet867, 2, 2
_PickedSet867, 6, 6, 2.5
**
** LOADS
**
** Name: Prepreg-1-Tension Type: Concentrated force
*Cload, follower
_PickedSet779, 3, -10.
** Name: Roller consilidation force Type: Concentrated force
*Cload
_PickedSet863, 2, -100.
**
** CONTROLS
**
*Controls, reset
*Controls, parameters=time incrementation
, , , , , , , 20, , ,
**
** OUTPUT REQUESTS
**
*Restart, write, frequency=0
**
** FIELD OUTPUT: F-Output-1
**
*Output, field, frequency=2
*Node Output, variable=PRESELECT
*Element Output, directions=YES, variable=PRESELECT
*Contact Output
CDISP, CSDMG, CSQUADSCRT, CSTRESS
**
** HISTORY OUTPUT: H-Output-1
**
*Output, history, variable=PRESELECT
*End Step
Regards, Kunming
The website is not allowing for uploading files. If it is applicable, could you upload it to any platform and send the link.
Many thanks for your response.
I see from the image you are sharing that the tape/prepreg is moving with the roller not sticking to the base.
This was one of my errors I was facing despite the existence of cohesive interactions.
@kmao24 it should allow you to upload files up to certain size (with certain extension). Can you let me know the error message while you upload files?
I compressed the file whose size is less than 0.5 mb. Then I run into this error:
“Sorry, new users can not upload attachments.”
I upgrade you to be a bronze contributor now. You should be able to upload file now.
j-model-1-mod-2step.zip (481.8 KB)
Thanks! It looks OK now.
