List node results and coordinates

[rcfanatic]

Hi everyone,

I began using ANSYS Workbench 12.1 recently, moving from ADINA. My question is in regard to post processing data. I have a part that flexes under a vacuum to create a bowl shape. I need to find the curve that represents the deflection at its center cross section. I assume I have to "section" the CAD part in Design Modeler first, so that I can mesh a line of nodes. Any tips on this would be great. However, I still don't see how I would display results for individual nodes once I have this step completed. Any input would be greatly appreciated!

Thanks,
Adam

 

[rcfanatic]

Update:

I now have my line of nodes. I was able to "slice" the part in design modeler. Although I couldn't find a way to sew, merge, connect, or unite the two halves, I used a bonding contacting region in Mechanical so it would solve the same as one part and the results came out correctly.

***So my only outstanding question is, how do I identify the node numbers on the cut edge, find their coordinates, and then list the deformation results for those node?

Thanks for any input!


Adam

 

[rcfanatic]

Anyone? I know there must be a way to do this

 

[flash3780]

You might check Roarks; I think that the case that you're trying to simulate can be solved analytically. That said, if you're trying to select and output nodes, you may find it easier in Ansys APDL.

To grab node locations and displacements from Workbench, you'll have to click "Tools>Options>Simulation>Export>Include Node Locations/Include Node Numbers".

From there, you can output nodal coordinates by right-clicking on your displacement results and selecting "Export".

To connect parts in Workbench, you'll select the parts that you want to share nodes in DesignModeler, right click and select "create new part". When you mesh your part in Simulation, it will then share nodes across cut boundaries. Cutting up parts and gluing them back together is very useful for creating efficient (brick) meshes. Contact elements should generally be avoided unless they're necessary for the simulation because they're slower and less accurate than a continuous mesh for most situations.

Check out the Ansys customer portal; they've got some great tutorials that you may find useful. Also, if you decide to take a crack at Ansys APDL, the help file has some great tutorials for that as well. Good luck.

//signed//
Christopher K. Hubley
Mechanical Engineer
Sunpower Incorporated
Athens, Ohio
--

http://engineeringliberty.wordpress.com

 

[rcfanatic]

Hi Christopher,

Thank you very much for your reply! I was able to export the nodes with their locations and values, but I don't know which node numbers are associated with the nodes I have created by slicing the model. I attempted to use the "xyz" tool in the graphics area but it is too cumbersome.

Is there a way to display the node numbers in the graphic area? If not, then what is the best way to import this solution into the APDL and use it for post processing?


Sincerely,
Adam

 

[flash3780]

You have to tell ANSYS to save the MAPDL database (it's under Analysis Settings>Data Management, I believe).

After you do that, you can resume the database and read the results in Mechanical APDL. From there, you can plot nodes (NPLOT) and diaplay node numbers. I'd recommend walking through a couple of the tutorials to get a feel for the user interface. Ansys APDL is a powerful analysis tool, but you have to invest a bit of time learning how to use it before you can utilize its potential. I find that it's best to think of Mechanical APDL as a high-level programming language (like Matlab, Mathematica, R, etc.) with a command line interface and some handy GUI tools.

//signed//
Christopher K. Hubley
Mechanical Engineer
Sunpower Incorporated
Athens, Ohio
--

http://engineeringliberty.wordpress.com

 

[rcfanatic]

Thanks again Christopher, I'll give that a shot. Mechanical APDL is very similar to ADINA in terms of it's power and learning curve. Out of curiosity, between MAPDL and Workbench, which is more commonly used in industry? Or does it just depend on the industry? With the limited post processing capabilities of Workbench is seems like it is good only for a visualization tool.

Thanks,
Adam

 

[flash3780]

Adam,
Good luck. Workbench isn't bad, it's just different. The geometry manipulation tools available in Workbench (DesignModeler) are great, and the latest version has quite a bit more flexibility and some exciting features which allow easy linking of different models, etc. Workbench has plenty of functionality for many users. Still, APDL rules the roost when it comes to capability, flexibility, and parametric modeling.

-Chris

//signed//
Christopher K. Hubley
Mechanical Engineer
Sunpower Incorporated
Athens, Ohio
--

http://engineeringliberty.wordpress.com

 

[rcfanatic]

After working through a couple tutorials and poking around I was able to list the results for the nodes and generate a curve for the window. Perfect!

When using PlotCtrls>Numbering>Node numbers, many of nodes have overlapping (superimposed) numbers and were illegible. Luckily, my line of nodes all had z=0 and y=0 coordinates so I was able to filter the listed results to find which ones I needed.

However, I am now working on a full vacuum chamber with many internal parts and therefore many superimposed nodes. Today I learned how to create cross sections, but when I choose Plot>Nodes it displays them for the entire model, not just the section. Do you have any suggestions for viewing nodes only in a section, or only on an exterior surface?


Thank you again!

Best,
Adam

 

[flash3780]

Adam, you can select only the nodes that you'd like to display. Try the node selecting tools in Ansys. The NSLA or NSLL commands can grab the nodes attached to an area or along a line respectively. It may also be useful to create components (CM), or groups of nodes, elements, etc which you can select at any time (CMSEL). Good luck.

-Chris

//signed//
Christopher K. Hubley
Mechanical Engineer
Sunpower Incorporated
Athens, Ohio
--

http://engineeringliberty.wordpress.com

 

[rcfanatic]

Chris,

Just to elaborate a little more, the way I am approaching these problems is to import a Solidworks model into Workbench, solve, then output and use the APDL for post processing.

The issue I'm running into is that since I created the model in Solidworks, there are no defined lines or areas that the APDL recognizes, so I cannot use NSLA or NSLL. Is there a way to designate lines and areas in the Design Modeler, so that they will be exported along with the solution? Or is there a reasonable way to define lines and areas within the APDL, using just the mesh/nodes that the Workbench exports?

Thank you again for your help and patience!

Adam

 

[flash3780]

Adam,
Your setup isn't ideal; geometry (areas, volumes, etc) is lost when a model is passed to from Workbench Mechanical to MAPDL. What you can do is define "Named Selections" in Workbench (which are the same as "Components" in MAPDL - see the CM command). You can then select the nodes attached to those "named selections" created in Workbench when you're in MAPDL with the CMSEL command (eg. "CMSEL,s,my_named_selection").

You can also use the selection tools (box select, etc) to select only the nodes or elements that you want... but that can be a bit tedious. Good luck.

Playing around with the selection tools and selection commands will go a long way towards making you more comfortable in the MAPDL environment.

-Chris

//signed//
Christopher K. Hubley
Mechanical Engineer
Sunpower Incorporated
Athens, Ohio
--

http://engineeringliberty.wordpress.com

 

[rcfanatic]

Chris,

I am working on a new steady state thermal analysis that I plan to try the named selections on. However, more pressing is that it will only output the temperature solutions and not the heat fluxes. In APDL I'm given the option to print X, Y, Z, or Vector sum but come up with this error when I choose any of them


*** WARNING *** CP = 40.576 TIME= 18:10:40
The requested TF data is not available. The PRNSOL command is ignored.


Is there a reason why Workbench would not output all the solutions in file.db?


Thanks!
Adam

 

[rcfanatic]

Does anyone know how to output the heat fluxes in a steady-state thermal solution to a MAPDL file?

 

[flash3780]

Try adding OUTRES,ALL,ALL to a command snippet in Workbench to output heat fluxes into MAPDL.

//signed//
Christopher K. Hubley
Mechanical Engineer
Sunpower Incorporated
Athens, Ohio
--

http://engineeringliberty.wordpress.com

 

[rcfanatic]

I inserted the outres command into both the solution setup and results (see image) but I still receive the same error when trying to read heat flux data from the *.db file.

 

[rcfanatic]

Here's the image, attached

 

[rcfanatic]

Hi Everyone,

I'm still on the same issue of outputting heat flux to an MAPDL file.

I need to integrate the heat fluxes over a cross sectional area in order to solve for the total amount of heat entering a system. I don't think there is a way to do this in ANSYS Mechanical, so I assume I must have to output the nodal results, list them in ANSYS APDL, and integrate from there.

Can anyone provide insite on how to output these results? I've tried the OUTRES command (see above) without success. I'm certain there must be a way to do this.


Thanks,
Adam

 

[sayuri]

I had same problem.

Add set,last in the beginning of your code.

After the function of that you are using for tf, write *stat
Like this (you can check this at output file)
*vget,QRes(1),node,1,tf,z
*stat,QRes
For my case, it works.
"apdl database is not holding the information that it should hold"
but with printing it, it holds.