Hello Goodat Crossfire ,

I have additional question: why exactly do you need movable datum CSYS?

Nevertheless, you can create additional datum CSYS directly in odb file.

In Visualization module go to Tools > Coordinate system > Create. Here you can create a new datum based on 1 or 3 nodes.

After that, you can go in Visualization module to Results > Options > Transformation. Here choose User-specified Transform Type, choose your new coordinate system and click on Include effects..., Primary variable and Deformed variable. After that your new datum CSYS will be the main one and all deformation will be shown around it.

Sincerely,

Pavlo

Hi all,

There is an option Creating a coordinate system following a single node:

https://abaqus-docs.mit.edu/2017/English/SIMACAECAERefMap/simacae-t-rescsyssinglenode.htm

Pavlo Pavliuchenko Hi, thank you for your answer.

I think the method you mentioned is performed in the postprocessing. However, my purpose is to build a coordinate system which can be moving with a certain part during the analysis( changed at each step and frame of the analysis). Imagine that when I build the coordinate system for a moving motor( the Z axis would be used as the rotation axis of the motor), it's necessary for the coordinate system to be attached/fixed to the moving motor. Otherwise, after some steps, the motor(which is moving with some other part) and the coordinate system (which is fixed) are not coincident, then it makes no sense.

Victor J. Аdlucky Hi Victor, thank you for the answer very much. I need the moving coordinate system to be functional during the analysis/simulation, not in the postprocessing, since the direction of load is dependent upon the coordinate system. Do you think is it possible to build a moving/adjustable coordinate system which will be used in applying the load?

Thank you!

Hi Goodat Crossfire,

You are right. Unfortunately, this method is intended for postprocessing. Moreover, it turnes out that datum CSYS are stationary. Maybe the next quotation from User's Guide will be helpful: "Connector elements defined without kinematic constraints or constitutive behavior can be used to monitor kinematic output in local coordinate systems. Quantities of interest include relative position, displacement, velocity, and acceleration in local coordinate parametrization. Finite rotation parametrizations include Euler and Cardan angles, rotation vector, and flexion-torsion-sweep. For an example that uses a connector element to monitor Euler angles, see “Motion of a rigid body in Abaqus/Standard,” Section 1.3.6 of the Abaqus Benchmarks Guide."

Hello Goodat Crossfire ,

I have done small investigation and found out that actually it is (could be) possible to perform your task using just one datam CSYS. But it is important how you define the motor/moving part displacement boundary conditions.

I created small example model with two parts: Motor (orange cylinder) and Housing (blue hollow cylinder) (assembly.png). Each of the parts contains one reference point (RP_Motor and RP_Housing). The reference point of part Motor is located at the rotation axis of the cylinder. The reference point of part Housing is shifted down by 100 mm from the rotation axis of the hollow cylinder.

Part Motor contains two surfaces: SideSurface and OuterSurface. Part Housing also contains two surfaces: SideSurface and InnerSurface.

In Assembly part Motor is placed inside Housing part. There is surface interaction between OuterSurface of Motor and InnerSurface of Housing (Hard, Frictionless).

Reference points of each part are constarined with corresponded SideSurface usind Coupling, Continuum distributing Constraint.

Boundary conditions:

*Boundary

Housing.RP, 1, 1

Housing.RP, 2, 2

Housing.RP, 3, 3

Housing.RP, 4, 4

Housing.RP, 5, 5

*Boundary, type=VELOCITY

Housing.RP, 6, 6, 6.28319

*Boundary

Motor.RP, 3, 3

*Boundary, type=VELOCITY

Motor.RP, 6, 6, -6.28319

The idea behind that boundary conditions is that Housing rotates around its reference point (RP_Housing) in counterclockwise direction and moves Motor, but Motor but also rotates around its reference point (RP_Motor) in clockwise direction. And it works. The rotation axis of the part is defined by position of reference point.

Ofcourse, I don't know the exact conditions of your model, but maybe it can help to solve your problem.

Sincerely,

Pavlo

Concerning moving coordinate system (MCS) used for applying the load. If we apriory know the law of movement of MCS and the loads which are given in it, we can express those loads in any convinient stationary CSYS via coordinate transformation and using abaqus amplitudes. Otherwice, if position of MCS depends on previous loading history, the user subroutins may be needed. Also note that many distributed loads in abaqus are follower, i.e. change its direction during deformation.

Pavlo Pavliuchenko Hi Pavlo, thank you so much for the insightful anwser.

I don't understand the code for boundary conditions your presented. But I can get the point you are trying to say that the rotation axis of the motor can follow the RP.

May I ask that is the innersurface of the housing and outersurface of the motor constrained with coupling or just contact? Is the rotation of the motor defined in the default/global coordinate system? Suppose that the motor rotates about the UR3 degree of freedom, then maybe the UR3 of the RP can change its direction with the motion of the housing (since the RP of motor is coupled with the housing) ?

Appreciate it very much! Thank you.

Victor J. Аdlucky Hi, Victor, yeah exactly, the direction of the load depends on the real-time deformation in every increment. Do you mean I can achieve this goal by using subroutines?

Intuitively, I think this is a common application and demand. I hope that Abaqus can do the job for me after some not-so-hard settings.

Thank you!

Hello Goodat Crossfire ,

I attach the pictures with boundary conditions and constraints.

Outer Motor surface and Inner Housing surface are not constrained at all. They just have surface to surface interaction.

I used everywere in boundary conditions and constraints in the model the default/global CSYS.

Basicaly Housing_RP is constrained from movement in any direction by boundary conditions, so I don't think it can changes its rotation direction.

Try to create the similar model by your own. If it will work, maybe it can help you with you main model.

Sincerely,

Pavlo

Pavlo Pavliuchenko

Hi Pavlo,

All is working fine because both axes of rotation remain parallel. But what happens if we want PR_Housing's rotation about, say, X axis ?

Hello Victor J. Аdlucky ,

yes, I understand that my approach doesn't solve all problems. I do not have now the model that should be simulated, so I just have given a hint that could help. Ofcourse, if the model rotates in any imaginable directions, my approach probably will not work. But again, I do not know the problem to give the exact answer.

In the end, maybe the using of subroutines will be anavoidable.

Sincerely,

Pavlo