Using User Defined Results in ANSYS Mechanical

By: Doug Oatis
– June 27, 2011
Categories:

I first started contemplating this article several weeks ago, and I was planning on somehow working in a Jersey Shore reference.  But now that I’ve relocated to Colorado and am recovering from a climbing trip that was a bit above my ability, my creative juices are a little low (they were used up trying to improvise my way up an overhanging roof pitch).

Hmm…I’m noticing there aren’t a lot of foot-holds to get me over there, prussik to the rescue!

Anyways, User Defined results were first introduced in R12 to grant the user access to element table items. 

When you insert a user-defined result, you are required to fill in the ‘expression’ line in the details window. 

Just like Johnny 5, ANSYS needs input

You can look up everything that’s available through the documentation, but we all know that no one reads the instructions

Reading is boring…I’ll wait until the movie comes out, I hear it stars the guy who voiced Johnny 5

There’s a much easier way to auto-populate the ‘expression’ line…the Worksheet view!  To access this, first click on the ‘Solution’ branch and then select ‘Worksheet’ (tab in R12, button in R12.1 and newer).  This will show you a list of all the user defined result expressions.  Find one you like, right-mouse-click on it and select ‘Create User Defined Result’. 

That’s more like it

This will insert a ‘User Defined Result’, the only work you need to do is scope it to a body (if necessary).  The only ‘tricky’ part of this process is that you need to solve the model first before using the Worksheet view.  This is because before the model has been solved, Mechanical doesn’t know what is in the result file.  So if the worksheet view is blank or grayed out, it’s because you haven’t solved the model.

So what’s the benefit of using the User Defined Results?  Say you wanted to look at total strain, kinetic energy, or reaction force contour plots…just to name a few.  In order to view any of those, you would either have to open the .rst file in MAPDL or use the User Defined Result.

Left = FX, Right = Total Strain

Here’s a quick description of the ‘headers’ available on the Worksheet tab.

UDisplacement
SStress
EPTOTotal Strain
EPELElastic Strain
EPPLPlastic Strain
EPTTThermal Strain
ENFOElement Nodal Reaction Forces
NDIRNodal Orientation Values

There are more headers that are listed in the documentation (I know, we all agreed that was boring).  However if you’re looking for items stored in the NMISC or SMISC (for ‘regular’ or contact elements), those are accessible provided you properly format the expression line.

So now let’s go through an example where we actually use this functionality.  A customer called in asking how to calculate the volume of a part above a specified stress level.  Interesting question…

First we create a user defined result and use the ‘VOLUME’ expression.  So we’re half-way there.  Next, we need to understand about how the results are stored for a result item in the ‘Solution’ branch.  Each contour plot is actually a vector in the form of element/node vs result.  You can see this for yourself by right-mouse-clicking on the item in the tree and selecting ‘export’.  So right now we have a vector defined of element vs volume.  Now we just need another listing of element vs stress.

When you create a stress result in Mechanical, the default behavior is to show the nodal-stress, which represent the average of the adjacent elements.  That’s not what we want.  If we look into the ‘Integration Point Results’ we see there are more options.  Element mean seems like it might work for us, but when we export it, we see that it’s still reporting stresses at the node, only now it’s using a different integration scheme.

Averaged
Elemental Mean

In order to access the average stress value of the element (not node), we need to use the User Defined Results.  We’ll ask to evaluate the expression seqv (von Mises) and set the integration option of using the elemental mean.

Now when we export that result item we get what we want…element vs stress:

Now we just need to export both vectors (volume and stress), then copy/paste/sort/sum and you’re done.  Don’t forget the most important step…billing for 4 hours of post-processing work.

Long story short, all you MAPDL users who have been complaining about not being able to access element tables should take a look at the User Defined functions. 

Categories

Certified Elite Channel Partner

Get Your Ansys Products & Support from the Engineers who Contribute to this Blog.

Product Development
Diamond Partner

Technical Expertise to Enable your Addictive Manufacturing Success.

PADT’s Pulse Newsletter

Keep up to date on what is going on at PADT by subscribing to our newsletter.


By submitting this form, you are consenting to receive marketing emails from: Phoenix Analysis and Design Technologies, 7755 S. Research Dr., Tempe, AZ, 85284, https://www.padtinc.com. You can revoke your consent to receive emails at any time by using the SafeUnsubscribe® link, found at the bottom of every email. Emails are serviced by Constant Contact

Share this post:

Share on twitter
Share on facebook
Share on linkedin
Share on pinterest

Upcoming Events

08/10/2022

Tucson after5 Tech Mixer: Ruda-Cardinal

08/05/2022

Flagstaff Tech Tour, 2022

08/02/2022

2022 CEO Leadership Retreat

08/01/2022

2022 CEO Leadership Retreat

07/27/2022

Thermal Integrity Updates in Ansys 2022 R1 - Webinar

07/20/2022

Simulation Best Practices for the Pharmaceutical Industry - Webinar

07/14/2022

NCMS Technology Showcase: Corpus Christi Army Depot

07/13/2022

NCMS Technology Showcase: Corpus Christi Army Depot

07/13/2022

Additive & Structural Optimization Updates in Ansys 2022 R1 - Webinar

07/07/2022

Arizona AADM Conference, 2022

06/29/2022

LS-DYNA Updates & Advancements in Ansys 2022 R1 - Webinar

06/23/2022

Simulation Best Practices for Wind Turbine Design - Webinar

06/15/2022

MAPDL Updates & Advancements in Ansys 2022 R1 - Webinar

06/01/2022

Mechanical Updates in Ansys 2022 R1 - pt. 2 Webinar

05/26/2022

Modelling liquid cryogenic rocket engines in Flownex - Webinar

05/25/2022

SMR & Advanced Reactor 2022

05/25/2022

05/24/2022

SMR & Advanced Reactor 2022

05/19/2022

RAPID + tct 2022

05/19/2022

Venture Cafe Roundtable: AI & Healthcare

05/18/2022

Tucson after5 Tech Mixer: World View

05/18/2022

RAPID + tct 2022

More Info

05/18/2022

Signal & Power Integrity Updates in Ansys 2022 R1 - Webinar

05/18/2022

Simulation World 2022

05/17/2022

RAPID + tct 2022

05/11/2022

Experience Stratasys Manufacturing Virtual Event

05/04/2022

Mechanical Meshing Updates in Ansys 2022 R1 - Webinar

04/27/2022

04/22/2022

12TH ANNUAL TUCSON GOLF TOURNAMENT

04/21/2022

04/20/2022

Additional Fluids Updates in Ansys 2022 R1

04/20/2022

Experience Stratasys Tour – Tempe Arizona

04/18/2022

Experience Stratasys Tour - Flagstaff Arizona

04/14/2022

D&M West | MD&M West

04/13/2022

D&M West | MD&M West

04/13/2022

Experience Stratasys Tour - Albuquerque New Mexico

04/12/2022

D&M West | MD&M West

04/12/2022

Experience Stratasys Tour - Los Alamos New Mexico

04/12/2022

Optimizing Engineering Workflows f​​​​or Propulsion System Design

04/07/2022

Experience Stratasys Tour - Austin Texas

04/07/2022

37th Space Symposium - Arizona Space Industry

04/06/2022

Transforming Digital Engineering with Ansys Discovery 2022 R1

04/06/2022

37th Space Symposium - Arizona Space Industry

04/05/2022

37th Space Symposium - Arizona Space Industry

04/04/2022

37th Space Symposium - Arizona Space Industry

03/30/2022

Simulation Best Practices for Vehicle Engineering - Webinar

03/23/2022

03/23/2022

High & Low Frequency Electromagnetics Updates in Ansys 2022 R1

02/24/2022

Arizona Technology Council After 5 Tech Mixer "Pandemic Pivot Pizza Pa

02/23/2022

SciTech Festival: Spend an Hour with 3D Printing Experts

02/11/2022

Webinar: Mechanical overview for Ansys 2022 R1

More Info

02/09/2022

Webinar: Product Development 101 (FAKE)

02/08/2022

Webinar: Navigating the Additive Landscape

01/27/2022

Arizona Technology Council 1st Quarter VIP Tech Mixer

More Info

01/26/2022

Simulation Best Practices for Gas Turbine Design & Development - Webin

More Info

01/19/2022

Arizona Photonics Days

More Info

11/04/2021

ExperienceIT, New Mexico

More Info

11/03/2021

Additive Manufacturing & Structural Optimization in Ansys 2021 R2 - We

More Info

11/03/2021

Optics Valley Technical Series: The Future of Simulation in the Optics

More Info

11/02/2021

SBIR Liftoff AZTC Virtual Breakfast Series

More Info

10/10/2021

Stratasys Mobile Truck Stop - Tucson Arizona

More Info

Search in PADT site

Contact Us

Most of our customers receive their support over the phone or via email. Customers who are close by can also set up a face-to-face appointment with one of our engineers.

For most locations, simply contact us: