ANSYS Workbench 14 Line Model Question

[jxsnyder]

I have recently been learning how to use ANSYS Workbench 14. I have been working through the examples outlined in "Finite Element Simulations with ANSYS Workbench 14" by Huei-Huang Lee. I am now working on a 3D building frame that utilizes different cross sections. In DesignModeler I added all of my points, created lines from points (added frozen), created cross section profiles, assigned the cross section profiles to the appropriate lines, and then selected all bodies and formed a single part. I then open up the system in Mechanical and apply my loads, fix my end connects, generate a mesh, and go to solve. I get the following error:

"Solver pivot warnings 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."

Please help!

Thanks,


Joshua

 

[0rel]

Hi,

If all of your bodies are in the same part, this is not a contact issue. Check your materials to verify that you didn't forget something. To see if your model is underconstrained, try running a modal analysis. 0-frequency modes (if you have some), will show you the rigid body motions allowed in your model, with that, you can set the missing BCs.

 

[jxsnyder]

So I went back and verified all the material is "structural steel". I then duplicated my static structural analysis and dragged/dropped modal onto solution. I then opened the model and proceeded to solve. I got the same warning as above and a new one:

"You have performed a pre-stress modal analysis with large deflection effects turned off in the static analysis. For a more accurate modal solution, we recommed turning on large deflection effects."

I turned large deflection to "on" and reran the solution. I now have the following two errors/warnings:

"An internal solution magnitude limit was exceeded. Please check your environment for inappropriate load values or insufficient supports. Also check that your mesh has more than 1 element in at least 2 directions if solid brick elements are present."

and

"One or more of your branches is dependent on a linked branch that is setup to solve remotely. The remote solutions for the linked branches have been started. You will need to retrieve the results for those branches and submit the solve request again for the remaining branches."

 

[0rel]

Drop the modal analysis on "Model", not solution, you don't need it to be pre-stressed.

 

[jxsnyder]

So I dropped it onto model and then had it solve. I have 6 modes of with frequencies of 0, 0, 0, 3.7479e-005, 5.0426e-005, and 5.0426e-005, respectively. Does this mean the system is not setup to act like a rigid body?

 

[0rel]

Did you re-apply your boundary conditions in your modal analysis ? It seems you only have rigid body motion.

Also, your model is not supposed to "act like a rigid body". A rigid body motion means your model is underconstrained. The modal analysis helps you see what conditions are missing. For example if you have a 0-freq mode with displacement in X-direction, it means you have no contrain in that direction. Thus here, I guess you have no constrains at all.

 

[jxsnyder]

On a different note, if I were to model the same system with all members being the same cross-section and when creating lines from points utilizing "add material", I do not run into the issues I am seeing above. I created all lines as frozen so that I can change the cross-sections (i.e. I-beam, HSS, etc). So what kind of BC's does Workbench apply automatically in that case versus adding lines as frozen?

 

[0rel]

If you select "add frozen", you add a different body, if not, the "material" is added to the existing body.

 

[jxsnyder]

If you select "add material" is there a way to change the cross-sections of the different members? From what I have seen it appears that it only allows you to choose 1 cross-section by doing that.

 

[0rel]

No, if you add material, you only have 1 body, and the cross-section is associated with a body. You need to create different frozen bodies.

But when you have all your bodies and cross section created, select your bodies in the tree, right click > form new part, your different bodies will be put in the same part, which is kind of the same thing but allowing you to have different cross sections (and also different materials etc...).

 

[jxsnyder]

That is exactly what I did for this project. I also tried creating the same system but instead added all of my lines as "add material" making a system entirely of one cross-section. Performing an analysis like this did not create any issues. With that system of one cross-section I did not apply any specific boundary conditions (fixed ends on columns to ground and applied loads). So what kind of BC's does Workbench apply automatically if your system is entirely the same cross-section? What kind would I need to apply for this? If interested, I can attach a screenshot of what I am working with a little later today.

 

[0rel]

Yes, the screenshot would help.

Workbench doesn't apply BCs depending on the cross section, only depending on how you define them in mechanical.

Do all your bodies' extremities coincide with at least one other body ?

 

[jxsnyder]

See attached. The four columns are HSS5x5x3/16, cross bracing are L5x5x5/16, and the beam with the 16000 lb applied load is S15x50. The rest are either W10x12, W12x16, or W12x26. All were added frozen and all bodies coincide with each other.

 

[0rel]

Did you form a single part with all your bodies ?

What you could try is to add bonded contacts where your bodies touch.

 

[jxsnyder]

I did end up selecting all bodies and created a single part in DesignModeler. When I go into the Model and try to apply a bonded contact it tells me that the scoping is set to manual and doesn't seem to work. Can you run me through how to apply the bonded contacts? Also, do I have to do anything special for where the cross bracing, columns, and beams come together?

 

[0rel]

Well unfortunatly I never used contacts with beams. I don't know why your model doesn't run and I lack the experience to have more ideas

Maybe, if your model is not confidential, you could upload it, I could try to find some time to look at it next week.

 

[jxsnyder]

Well I had a big "aha" moment and realized that I made line bodies from column to column. I changed it to seperate line bodies between the joists and the system now works! Thank you for your patience and help. I greatly appreciate it!