## General Mechanical

Topics relate to Mechanical Enterprise, Motion, Additive Print and more

#### Getting a solver pivot warning or error. not sure what this means and why am i getting this?

• moawezawan
Subscriber

Hi! I am trying to carry out a static analysis on a load bearing bar that holds an antenna dish. I apply pressure force on the flat plate and two rings. I am not sure why am I not being able to solve this. Please help! thanks!.jpg?width=690&upscale=false" alt="">

• peteroznewman
Subscriber

How many solid bodies are there in the Geometry tree?

If there is more than one solid body, then the error is because the bodies are not connected.

This ring doesn't seem to be connected to the bar. Those two meshes just seem to overlap one another.

.jpg-(1920×1080).jpg?width=690&upscale=false" alt="">

Go back to CAD and Unite those two bodies if they are the same material.

If they are different material, then you need to Boolean subtract the bar (keep tools) from the rings. Then you can connect them using Shared Topology or Bonded Contact.

• moawezawan
Subscriber

Hi Thank you so much for your reply! I have four different geometries joined together. The materials im using are two different ones. I have tried to join the parts together again but I am still getting the same error. Can you tell me whats the issue still? Thanks again!

• peteroznewman
Subscriber

None of your screen images show what is in the connections folder. That is where the problem will be resolved.

Use File, Archive to create a .wbpz file to attach after you post a reply.

• moawezawan
Subscriber

Hi! I am uploading a wbpz file  with this message. Hope you can shine some light on what is the issue. Thanks!

• peteroznewman
Subscriber

The geometry still has overlapping (interfering) solids.

Go back to SpaceClaim and use the Combine Tool to Add three solids to the first one, then there will be a single solid body.

The problem you will have is exceeding the allowable Node count of 32,000 on the Student license.

As you can see, the default mesh has exceeded that limit.

If the load is symmetrical, you can use Symmetry to cut the model size in half. Since the face with the pressure got cut in half, you get half the force. But if you had applied a force, you would have to type in half the value for the force. You have to right mouse click on Model and insert a Symmetry folder, then right click on the Symmetry folder and insert a Symmetry Region, select the face and set the normal to be the Y axis.  Now the mesh size is below the limit.

If the load is not symmetrical, then you can convert some of the geometry into midsurfaces and use contact to connect the solid body ends. That is quite a bit of work in SpaceClaim.

The load you have is a pressure. Since there is an area, that creates an unknown force.  You can find out the force by clicking on the face and getting the area, or requesting a Probe > Reaction Force in the Solution.

• peteroznewman
Subscriber

After I solved the model, I wondered why there was such a large deformation and such a small stress.

The material used called "Steel" has a Young's Modulus of 0.207 MPa.

The Structural Steel that is available has a Young's Modulus of  200000 MPa.

Your Steel is off by a factor of one million.

I went looking for "Steel" in Engineering Data, but it's not there, it was defined in SpaceClaim.

Put six more zeros at the end of the Elastic Modulus.