Changing Results Values in ANSYS Mechanical APDL–DNSOL and *VPUT

By: Eric Miller
– March 30, 2012
Categories:

So it is Friday afternoon and that big, involved, deep-dive into some arcane ANSYS capability is still not written.  So, time for plan B and the list of not so involved but still somewhat arcane capabilities that we like to expose in The Focus.  At the top of that list right now is how to change the results in an ANSYS Mechanical APDL (MAPDL) solve. 

One might ask why would you want to do this?  Well the most common usage is that you want to use APDL to calculate some result value and then display it in a plot.  Similarly, you may want to do some sort of calculation or post processing on MAPDL results but using and external piece of code, but still show the results in ANSYS.  Another common usage is to use MAPDL as a post processor for some external solver. 

And, it turns out, it is pretty easy.  And, as you probably have learned by now if you use MAPDL a lot, there is more than one way to do it.

The “Database”

Before we get into how to do this, we need to talk about the “database” in MAPDL. If you read through the documentation on the commands we will use, it will talk about the database.  This is not the jobname.db file.  That is the db file.  The database refers to the representation of your model, including results and the currently active loads, in memory when you are running MAPDL. 

When you do a RESUME command, MAPDL reads the DB file and stores the model, including geometry, mesh, loads, and run parameters, in memory.  When you do a SET command, it then adds the results and related information into memory. 

So when we use the commands we will talk about next, you are changing what is in the database, not what is in the DB file on your disk.  And you are storing it temporarily.  Many different commands cause the database to go back to its original values.  So you need to be very careful in how you use these tools, and don’t assume that once you have used them, the changes are permanent.  

DNSOL

The simplest way to do it is with the DNSOL command: DNSOL, NODE, Item, Comp, V1, V2, V3, V4, V5, V6

So, if you do a dnsol,32,u,x,3.145  the value in memory for deflection in the X direction will be changed to 3.145.  dnsol,32,s,x,1.1,2.2,3.3 will change the stress on node 32 in the X direction to 1.1, in the Y direction to 2.2, and in the Z direction to 3.3. 

The second argument can also be a component, so you can assign a uniform result value to many nodes at the same time. 

Here is an example, very simple, of a block where we set the deflection on the top nodes to 1 in.

   1: finish

   2: /clear

   3: /prep7

   4: blc4,-2,-2,4,4,20

   5: et,1,185

   6: mptemp,1,70

   7: mpdata,ex,1,1,20e6

   8: mpdata,nuxy,1,1,.23

   9: mpdata,dens,1,1,.001

  10:  

  11: vmesh,all

  12: /view,1,1,1,1

  13: /vup,1,z

  14: /RGB,INDEX,100,100,100, 0

  15: /RGB,INDEX, 80, 80, 80,13

  16: /RGB,INDEX, 60, 60, 60,14

  17: /RGB,INDEX, 0, 0, 0,15

  18: /show,png

  19: eplot

  20:  

  21: nsel,s,loc,z,0

  22: cm,nbt,node

  23: d,all,all

  24: nsel,s,loc,z,20

  25: cm,ntp,node

  26: f,all,fx,10

  27: f,all,fy,12

  28: allsel

  29: save

  30:  

  31: /solu

  32: solve

  33: finish

  34: /post1

  35: plnsol,u,sum

  36:  

  37: dnsol,ntp,u,y,1

  38: plnsol,u,sum

  39:  

  40: /show,close

 

 

aa1003The Fancy Mesh

aa1004The Normal Solution

aa1005Solution with 1” deflection DNSOL’d onto the top nodes

Pretty simple. 

NOTE: One key thing to remember is you can not use this with Powergraphics. You must have /graph,full turned on.

*VPUT

The DNSOL is great for a few nodes here and there, or a constant value. But it makes for a big nasty *do loop if you want to do a lot of nodes. So ANSYS, Inc. give us the *VPUT command:

*VPUT, ParR, Entity, ENTNUM, Item1, IT1NUM, Item2, IT2NUM, KLOOP

As you can see, this command has a lot of options, so read the Help before you use it. Most of the time you have an array that stores the value you want stuck on your model in an array (ParR).  Then you specify what MAPDL result you want to overwrite and it takes care of it for you.

*vput,nws1(1),node,1,s,1 will place new values for maximum principal stress on all the nodes covered in the array , starting at 1. 

Here is an example of the code, after the same solve as above, to do a *vput instead of a DNSOL:

   1: finish

   2: /post1

   3: plnsol,u,sum

   4:  

   5: *get,nmnd,node,,num,max

   6: *dim,nwux,,nmnd

   7: *do,i,1,nmnd

   8:     nwux(i) =  i

   9: *enddo

  10:     

  11: *vput,nwux(1),node,1,u,x

  12: plnsol,u,sum

aa1017

The code places a displacement in the X direction equal to its node number.  So node 80 has a UX of 80. 

A key thing to note with *vput is that it is much more transient. Pretty much any other command that involves anything other than plotting or listing blows away the values you assigned with *VPUT.  So we recommend that you do a *vput before every plot or listing you do.

Thoughts, Questions, and Conclusion

Of course you should never use this to fudge results. 

You can get very fancy with this. When I use it I often turn off all the plot controls and then create my own legend. That way I can put hours of life on as temperature or SX and then make my own legend that says LIFE or something of the sort. 

Another thing to note is that if you DNSOL or *VPUT a displacement, then ANSYS will distort your plot by that much.  That is OK if you are changing deflection, but not so good if you are plotting life or some esoteric stress value.

A common question when you play with these commands is if you can store the modified results in the RST file.  You can for degree of freedom results, but not for stresses.  You use LCDEF and RAPPND. 

And what about ANSYS Mechanical?  Well it works totally different, and better. You can do all of this using Design Assessment, which was covered in a webinar and a Focus article you can find here.

The key to using these two commands is pretty much the same as any APDL command: Start on a small test model, write a macro to do it, and keep things simple. And, read the manual.  Everything you need to know is in there.

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

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: