Learning Forum

[RobertoLucena]

Hi, i´m working on a project that is necessary to get the bending stress of a shell, but occurs this error:

"For this result, the scoped geometry(s) or named selection should have at least one sheet or a face on sheet or a solid with solid shell mesh."

What I can do to fixe it?

 

[peteroznewman]

I expect you have a solid model of a thin-walled, shell-like, structure, and you have brought that solid model into Mechanical, meshed it, applied loads and supports and solved.  Please reply and insert an image of your geometry.

RMB on Mesh and Show > Sweepable Bodies.  Does the solid turn green?  If so, you can sweep through the thickness and assign SOLSHELL190 elements. You must assign a Method > Sweep to the body and on the Src/Trg Selection, set it to Manual Thin, then pick the face(s) on one side of the thin walled solid. Then on the Element Option, pick Solid Shell.

If the solid body is not sweepable, you have to go back to the Geometry environment and create a midsurface model of the solid body. That replaces the solid body with a sheet body that gets the thickness of the solid assigned as a property of the sheet body. That only works if the solid body has a uniform wall thickness. If the thickness varies, you should make it sweepable and use SOLSHELL190.

Regards, Peter

[RobertoLucena]

Hello Peter,

Thank you for the fast answer.

I will upload my geometry as requested:

I applied the Method> Sweep as told but occurs another error on the solution:

"A result is invalid with the current output control settings."

I did something wrong?

 

[peteroznewman]

Please attach a Workbench Project Archive .wbpz file to your post above.

[RobertoLucena]

Hello Peter,

How I attach the file here?

[peteroznewman]

On the right of your post above are five grey buttons. The last one is Attach. Then a browse field opens up and you select the file and click the Upload button.

[RobertoLucena]

Thank you! Finally found that bottom

I already attach the file above.

[peteroznewman]

I see your model with Solid Shell elements using ANSYS 2019 R1.

To get the Bending Stress to calculate, you have to turn on all the Output Controls and under Analysis Data Management, you have to Save MAPDL db set to Yes.

But do you know what direction the Local Element Direction 11 is pointing?  You need to know that. Well, here it is. The red arrow is 11 and it looks like a mess, right? I suggest you make a cylindrical coordinate system and override the element coordinate system as described in this post.

I don't understand why you have the bottom edge to be fixed, while the top edge has a line pressure.

If you have something fixed and you push on it, nothing happens, so I think your line pressure is not doing anything. In fact, if I suppress the line pressure, I get the same result.

What kind of edge constraint did you want on the plate?  Did you want it clamped or pinned?  In other words, did you want the rotation fixed at zero on the edge or did you want to allow the edge to rotate about a hinge on the edge?

[RobertoLucena]

Hello Peter,

Lets go by parts:

1- I change the output controls and analysis data management and really works! Thank you a lot.

2 - About the cylindrical coordinate system, i had created the system but i dont understand why isnt applied to the model, i follow the steps of the topic that you recomended but i didnt find the modal branch

3- I´m studying a circular slab with the pressure of the water on the top. At the same time, i´m trying to simulate the Winkler soil (using elastic supports) at the bottom, but for some reason the software does not allow the simulation this way, so i put the fixed support (just on the edges) only to see what happened and guest what, work it (I dont no what i´m doing wrong, i will copy the errors that occurs without the fixed support):

a) "Solver pivot warnings or errors have been encountered during the solution.  This is usually a result of an ill conditioned matrix possibly due to unreasonable material properties, an under constrained model, or contact related issues.  Check results carefully."

b) "Not enough constraints appear to be applied to prevent rigid body motion.  This may lead to solution warnings or errors.  Check results carefully."

c) "A solver pivot warning or error has been detected in the UY degree of freedom of node 294 located in Solid. This is usually a result of an ill conditioned matrix possibly due to unreasonable material properties, an under constrained model, or contact related issues.  Check results carefully. You may select the offending object and/or geometry via RMB on this warning in the Messages window."

d) "Solver pivot warnings or errors have been encountered during the solution.  This is usually a result of an ill conditioned matrix possibly due to unreasonable material properties, an under constrained model, or contact related issues.  Check results carefully."

[peteroznewman]

You put the Command Object under the Static Structural (instead of Modal).  I repaired your Cylindrical Coordinate System to put the origin at 0,0,0.  Now all the Local Element Direction 11 points radially.

Add two planes of symmetry in DesignModeler. That will let you delete the Fixed Support and have no errors. Now the line pressure around the outside edge depresses the edge into the elastic support while the center depresses less.

Is the line pressure on the outside edge of the circular slab representing the weight of the wall? If that is the case, you should model the wall as well because that adds considerable stiffness to the edge of the base and doesn't allow it to bend as much as the slab model is bending.

[RobertoLucena]

Hello Peter,

You save a lot of my time, i probaly take weeks or even months to get at this point! Thank you very much!

I will try to repeat all these steps again tomorrow to see if i can get the same results, because i still have to do similar simulation in diferent situations.

The line pressure in the edge is for simulate the wall above it (it is a water tank storage)

I have some finals questions:

1- Why adding the symmetry allowed us to delete the fixed support? 

2- The primary reason for my work is to obtain the efforts (like moments and forces), it is possible with Ansys? or just give us the stress/strain?

 

 

[peteroznewman]

You should model the wall of the tank as well as the bottom slab because the wall adds considerable stiffness to the edge of the base and doesn't allow it to bend as much as the slab model with no wall is bending.

1. All Static Structural models need to be fixed in 6 DOF. The two Symmetry planes take away 5 DOF, leaving only the elastic support to control the Z axis.

2. Once the 3D model solves, you have stress through the thickness of the structure, but you can convert stress to force by multiplying by area.

If the posts above answer your original question, you can mark that post with Is Solution to close this discussion. You can open a New Discussion to ask new questions. You can show your appreciation by clicking Like on the posts that were helpful.