Learning Forum

[zjuv9021]

Hi all,

I'm simply looking for some assistance on how I can set up my BC's in order to put this tubing in stress states at a variety of angles (eg. 15, 30, 45, 60), as is displayed in the diagram below:

Please see attached .wbpz.

If i do a remote displacement, it just is rotating the face of the end of the tubing.. is there a way I can simply rotate about the end of the plank so as to make that portion completely straight and rotate the remainder of the tube 'x' degrees downward?

In essence, given the material behavior and other aspects of this tubing, how can I go about making it completely straight at or around 'x' degrees? As you can see above, the end isn't completely straight with the displacement I've given it.

Regards,

Zach

[peteroznewman]

Zach,

The reason you are not getting a straight tube at the lower right "red" end of the tube is because you have a BC that requires zero rotation about X.

Change the 0 degrees to Free on the Rotation X and it will allow the end to "straighten out".

Or require the 45 degree angle that you want, which is a negative rotation for this Coordinate System.

Regards,
Peter

[zjuv9021]

Thank you, Peter.

Do you know how I would set up my BC's in order to rotate my entire outer tubing so that it is 'x' degrees? Please see below for test fixture I would like to emulate. (Please also see attached .wbpz)

I would then like to push on the inner tubing so that it moves frictionless through the outer tubing.

Kind Regards,

Zach

[peteroznewman]

Zach,

I added an outer tube (green) that I set to be rigid (to reduce computational time solving) and added contact between the outer and inner tube.

I put a Revolute Joint on the outer tube, rotating about a point half way along where the Coordinate System is shown. I had a Joint Load of 45 degrees.

After 1 hour and 20 minutes of computation on 4 cores, this is the result.

A Translational Joint between the outer and inner tube can then push the inner tube in Step 2.

Attached is an ANSYS 19.2 archive.

Regards,
Peter

[zjuv9021]

This helps tremendously for my particular problem. I was not familiar with joints and how they operate. Thank you so much, Peter!

Regards,

Zach

[zjuv9021]

Did you taper the outer tubing to reduce high stresses at the 90 degree corners? And just one more thing, could you just provide an example of how I could effectively push just the inner tubing through this rotated plane back towards the fixed support?

Kind Regards,

Zach

[peteroznewman]

I put a radius (blend) on the edge of the outer tube to help the contact algorithm. It does better with face-to-face contact than face-to-edge. You might want to do that to the shelf the inner tube is pushing against. I asked for a 10 mm push in the model below, but the solver stopped with errors after only 1.1 mm.  You will have to improve the model to get it to solve further, but your request was for an example of how to push and it is simply to add one translational joint and load.

Regards,
Peter

ANSYS 19.2 archive attached.

[peteroznewman]

Hi Zach, please copy paste the above paragraph into a New Discussion in this Category and delete the above post.

The above discussion is marked "Is Solved" which means some people may not look at the new posts.

Regards,
Peter