Catia Fea retaining a pin 1

[engjeff]

I have a pin that goes through two bushings on the sides of another bushing.

The problem is the pin shoots out of the bushings.

I am able to apply a contact restraint with a clearance on the inner faces of the bushing to the pin.

But, If I try to restrain it the outer face of pin to outer face of bushing with a smooth connection over a general connection with a handler point (located in the center) the stress on the whole assymbly ends up in that location (not realistic).

How should you define a pin you want to stay inside of a bushing for Catia?

 

[fl11]

engjeff,

Does the pin shoots out axially of the bushing?

Again, dou you have a picture of the assembly of the pin?

Usually, what I do for an assembly pin/bushing, is to define a contact between the inner face of the bushing to the outer face of the pin. Then, restraint one of the side faces in axial translation and rotation. Therefore, all degrees of freedom are taken care of. In principle, those two restraints should not react any loads since they are there only to prevent rigid body motion of the pin.

 

[engjeff]

Fl11,

Thank you for your help, I attached a picture.

WHen you say you define a contact between the inner face to the outer face do you do that with a general connection? and if so then what connection do I define the general connection as?

Yes the pin is shooting out axially, if I constrain axially it expands in all directions.

 

[fl11]

ok, I am guessing that the three contacts we see in the pictures are between the pin and lug (middle one) and pin with bushings (two extremities). I picture of the assembly with transparent parts would also be usefull to see how everything is assembled. Can you send a picture with the results?

Anyway,

I would personally create a general analysis connection between the outer face of the pin and the inner face of the bushings. I would do the same thing for the lugs as well if I understand correctly the picture.

I would then define the contact property. Are the geometry designed at nominal dimension with interference or gap? If yes, then stay away from the clearance value. If the geometry were designed so the diameter of the pin is the same as the inner diameter of the bushing, then yes, a clearance value must be input.

Then, create a rigid virtual part on one side of the pin. Restrain this virtual part in axial translation and rotation. That way, all degrees of freedom are taking cared of.

It should work perfectly as long as a contact is detected between the pin and the bushing.

Once you have run it, see with a reaction sensor if the contacts and restraints transfer any loads. The contact should, but the restraints should not.

When you say the pin expands in all direction, is it at amplification magnitude 1? Sometimes, when you look at a higher amplitude, it seems like something is expanding, but it isn't in reality.

If it does not work and if you would like, you could make a little word document with more pictures showing how it is assemble and maybe, I could try to reproduce it on my part. To see how to do it.

 

[engjeff]

fl11,


The solution worked great, I do not know how to thank you enough!

On the clearance does the rule put clearance in when there is none and leave clearance out when there is real clearance hold true on a face to face clearance as well?

If so I assume the clearance button is actually for finding the most optimal clearance value without adjusting the model?

Thank you so much again.

 

[fl11]

In principle, the clearance value is there in order to create an artificial clearance or interference, without taking the geometry into consideration.

This means that even if the two geometry has an interferance, if you specify a clearance, it wont considerate the interferance. Works pretty greate.

 

[engjeff]

fl11,

After taking all the clearance off of the assybly's contact I keep getting error

FACTORIZATION FAILED IN CONTACT COMPUTATION
ABSOLUTE PIVOT NUMBER 3762 IS NEGATIVE OR NULL

VALUE : -7.03474E-015
POSSIBLE CAUSES:
1.CONTACT ELEMENTS ARE COINCIDING
2.A CONTACT ELEMENT IS CLAMPED

 

[fl11]

Ah, that error just drives me crazy! I honestly don't know for sure how to get rid of it, but usually, playing around with the mesh eliminates it.

Just try to make sure that no element that is part of the contact definition has something else defined on it (example, element is defined being in contact with bushing and rigidly connected with something else.)

I don't know hoe much contact connection you have, but I wuld suggestion that you define a rigid connection instead of contact for each of the contact. Then, transform them one by one into a contact while running the model at each step. That way, you will know with contact is problematic. (You can try to run it with TET4, it will go faster.)

If you double click on the mesh, then select the "selection" tab and you will see the contact definition (like contact 1.1). Pick them and place them in the box at the botton by clicking the single arrow. THis will plot on your screen all the contacts link. Look to see if something look weird.

Other than that, it becomes complicated to debug the problem without seeing it for real.

Let me know if you figure something out.

 

[engjeff]

That also helped alot I found a lot of errors... we are running the solution again. Thank you a lot, I will let you kow how it turns out.

 

[engjeff]

fl11,

Everything is working great! Thank you again for your help it was invaluable.

Jeff