Cylindrical constraints in Ansys

[edebs71]

Hi,

I'm trying to simulate a 2D rotating disk on a polishing Jig.

I created and meshed the disk (hollow disk). I rotated the nodes to Active cylindrical coordinate.

1. I applied Ux = 0(radial coordinate) on inside circumference of the disk.
2. I applied global acceleration
3. ran a transient analysis for 0.5 seconds.

The disk did not move at all, it seems that ansys does not understand radial constraints (it asigns the constraints only in the X direction not radially)

Could you please tell me what am I doing wrong.

thank you in advance.

 

[Drej]

ANSYS understands radial constraints perfectly well. Did you rotate all of the nodes into the cylindrical system, or just the ones that you wish to apply the radial constraints to? The latter would be the correct way to do it. Did you do a visual check to see whether the constraints have been applied correctly by yourself? Did you inadvertantly apply the constraints to ALL nodes in your structure? Have you checked the nodal reactions to see where exactly your model is constrained?

 

[edebs71]

thank you for replying,

I rotated all nodes into the cylindrical system (is this correct?)
I only applied the Ux=0 constraint to the inner circle

What am i missing?

 

[Drej]

"I rotated all nodes into the cylindrical system (is this correct?)"

No. As my post says, only rotate the inner circle nodes and apply your radial constraint here.

 

[edebs71]

thank Drej,

I did that (rotated only the inner circle nodes and applied the radial contraints. I appplied a global angular acceleration of 3.14 rd/sec^2 on the disk and ran a transient analysis for 0.5 seconds. When I checked the position of a specific node on the disk (it didn't move at all).

I animated the result over time (the disk didn't rotate at all).

I've tried the same procedure on a model moving in a straight line (X-direction) and everything looks OK (the model moved during this 0.5 seconds as it is supposed to).

Please help.......

 

[Drej]

How have you applied your loads (did you use ACEL or the DOMEGA command or what...?). I don't think you can apply an acceleration within ANSYS as a transient load, as acceleration is a body force. (ACEL is an inertial load, as is DOMEGA, rotational acceleration.) In some FE packages you can apply acceleration as a base excitation but not explicitly in transient form within ANSYS. Valid transient (structural) loads are displacement, force or derivatives thereof (e.g. pressure). If you have a rotating disk, why not analyse it statically using the DOMEGA command, or integrate your loads twice and use displacement. What does your transient input data look like? Is it time-acceleration?

 

[edebs71]

Drej,

I'm applying the acceleration DOMEGA as a stepped load in the transient analysis. Normally the disk should start rotating 'till it reaches a OMEGA = DOMEGA * time.

I tried a solid disk (constrain its central node radially) and applied the angular acceleration for 0.5 second as a stepped load. The disk started to rotate but the final rotation did not coincide with:
Theta = 0.5 * DOMEGA * time^2 + OMEGA(i)* time + Theta(i) (in this case OMEGA(i) and Theta(i) = 0)

Something doesn't make sence here (I don't think I'm missing any required step)

Any thoughts?

NOTE: I ran another transient analysis:

a) Load Step1: I specified a rotational displacement on the inner node during time t, to get an initial rotational velocity.
b) Load Step2: I removed the Uy constraints and ran for another T = 1 second

Ran an animation to see if the disk will continue to move(at the speed calculated from Load Step1) after Load Step 1 and guess what it didn't.

I thought that ANSYS could handle something like that easily.

 

[Drej]

"Any thoughts?"

Why do you need to run a transient analysis for this type of loading? My thoughts (as before) are: that you CANNOT use DOMEGA within a transient analysis and expect to see your disk rotating. If you want to analyse acceleration ONLY, I would use DOMEGA as a 'static' load applied within a static-type analysis. Why do you need to model the acceleration as a transient anyway? it doesn't make sense to me (maybe you have a simple explanation for this?). You will not see the model rotating because that is not the nature of the usage of this command. This command issued within a static analysis (ANTYPE,0) will give you what you need. What you should see here are stresses in the disk due to centripetal forces. Although this command is very much valid for transient analysis (for example, as a constant throughout loading), using this command in the way you have described is meaningless, and I would reconsider your strategy.

Cheers,

-- drej --

 

[edebs71]

Drej,

I'm trying to analysis the stresses induced in a Silicone Chip resting on a polishing disk as it accelerates from zero speed to a specified one at time T).

that is why I need the acceleration in a transient analysis.

Thank for your help,

Elias