# Same pressure applied in opposite faces

• 128 Views
• Last Post 09 October 2018
• Topic Is Solved
RetroBJJ posted this 05 October 2018

Hello everyone!

I just want to ask about my problem, which is related to excavations, open pit mine stability, etc. Geomechanics in general. There's something called in situ stress, and below ground it exists. These are applied at opposite faces of our model, and have the same magnitude at opposite faces of the outer boundary of the model. (See pic attached)

So basically, I need to apply a compressive pressure in a face x with magnitude X, and in the opposite face I need to apply THE SAME pressure. Same procedure needs to be followed for the rest of the faces of the box.

The issue is that, they seem to cancel to each other, so the final model is like it was never under the action of in situ stress, and only under the effect of gravity... Is there a way to fix this? it's really frustrating, because I am not getting the results I am supposed to get.

Cheers and thanks in advance. Hope you get my problem.

Attached Files

peteroznewman posted this 05 October 2018

Hello Retro,

The good setup is to take a cube, and on three faces, apply a displacement constraint with zero displacement in X on the face normal to the X axis, a zero displacement in Y on the face normal to the Y axis, and a zero displacement in Z on the face normal to the Z axis.  Now you have a cube that isn't going anywhere.

On the opposite face to the one that had the displacement constraint, apply a pressure. The reaction force on the face with the displacement constraint will have an equal and opposite force to the face with the pressure applied.

Let's say Z axis points up and gravity is working in the -Z direction. If you are doing it right, the pressure on the side walls should be a function of Z.

Regards,
Peter

• Liked by
RetroBJJ posted this 06 October 2018

When I first read your comment, it made me a lot of sense, in terms of physics. But as you may know, in other softwares this situation is a bit different (in ABAQUS for example, stresses don't cancel each other out when applied at faces).

I recently have made other simulations, but the results I'm getting aren't the expected ones.

It's supposed to have increased displacements in the inner part of the excavation, but the image attached doesn't show that sadly. I know that in this case the model is symmetric and I could have the desired results by cutting it in half, but that's not the idea... I want to know the general procedure to model this kind of situation.

I've tried with fixed boundaries, zero disp BC, etc. Any other advice dear Peter?

Have a nice weekend.

ps: Another question... is there a way to change the angle from radian to degrees in the engineering data? I have friction angle in radians and that's weird to me.

Attached Files

RetroBJJ posted this 08 October 2018

Good afternoon,

Is there a different way to proceed in this case? please, this problem is truly taking my sleep away.

peteroznewman posted this 08 October 2018

Retro,

I don't know what you were expecting with the attached image, or what you meant by "It's supposed to have increased displacements in the inner part of the excavation", maybe you could explain it in more detail.

If you want to upload a Workbench Project Archive, I will look more closely at your model.

Regards,
Peter

RetroBJJ posted this 08 October 2018

Peter, thanks again for your time and efforts in helping me.

When I said "increased displacements in the inner part of the excavation" I meant that the right simulation would have given me a displacement contour where vectors have direction towards the free faces of the excavation, so it's like the excavation shrunk (the technical term is convergence). The rest of faces have to remain without displacement (outer part of the box). In consequence, the highest displacements occur near the excavation.

Also, the min and max principal stresses should always be concentrated around the excavation (induced stresses), like in this example (keep in mind that this is not the same project, just an example to illustrate the idea):

And well... that's it. As a remainder, this is a cube (box) with an excavation (mining stope) inside and is under the action of s1, s2 and s3 compressive stresses just like this image below. And, the boundaries of the box should be constrained to have zero displacements.

The issue is that these stress cancel each other out if I model this situation as in other softwares. I hope now you can understand what I meant.

My project is attached, dear Peter. Thanks again for everything.

peteroznewman posted this 09 October 2018

Dear Retro,

Here is what I wanted you to do. For the Y face, set the displacement in Y to 0 while leaving X and Z free.

What you did was set all three to zero like is shown below.

If you make the same change for dx and dz, setting just one component to zero while leaving the other two free, you will get the following result.

If you plot the Y displacement, you can see the Average is -93 mm.

So if instead of Y = 0 you set Y = 93, then the center of the cave will have zero displacement and the cave walls will collapse in. Do the same for the X and Z axis.

I hope you like this.

Regards,
Peter

Attached is a zip file with an AIM 19.2 project

Attached Files

• Liked by
RetroBJJ posted this 09 October 2018

Hello again Peter, that looks a lot better! thanks for your kind support.

But... the displacement doesn't seem right to me. Is there a way to change this?

Ideally, higher displacements should be near the excavation, while the outer part of the box should be zero. I understand that what we got is an obvious result of the boundary conditions applied...so, by following this procedure should I renounce at looking at the deformation? (1)

A second question Peter, to finally close this topic... in the 'engineering data' in the material library, I have friction angle in radians and I can't convert it to degrees. Is there a way to change it? because I have that cell in gray, and in the unit systems I don't see the option :S (2)

Also, I don't understand why this value is also so low... 0.01 rad is like 0.57 deg, which is non realistic for the materials that I am aware of.

Thanks again, kind regards.

RetroBJJ posted this 09 October 2018

Peter, you have been so helpful... can't thank you enough for all this! as you can see, I am pretty newbie with Ansys.

Here's a z direction plot:

It makes sense... the only thing I am missing is how to display the vectors here.

Thanks so much.

peteroznewman posted this 09 October 2018

1) Plotting strain is the best way to see the local deformation in the material. Don't focus on the displacement because that just increases linearly from the point that didn't move, so the magnitude is not that useful.

2) You are stuck with radians for that field. Other places in ANSYS you can use degrees.  I don't know much about Mohr-Coulomb material model so I can't comment on the magnitude of that parameter.

Good Luck and Cheers,

Peter

• Liked by
RetroBJJ posted this 09 October 2018

Peter, thanks so much for all your time and kind support.

Have a fabulous week!

Best regards,

Retro