# Retrieving Accurate PSD Reaction Forces in ANSYS Mechanical

Categories:

We just finished up a tech support call for a customer that wanted a way to get accurate reaction loads from a PSD run in ANSYS Mechanical. Alex Grishin took the call and provided a nice example to the customer, so we thought we would leverage that and share it with all of you.  Even if you are not in need of this particular function, it is a great example of using snippets.  If you are not familiar with this, check out our recent webinar on the subject.

The reason why you have to do this is because doing an accurate PSD force calculation is not a simple thing.  The math is a bit complicated, because PSD responses are probabilities of results that loose sign.  And it is right now only available in Mechanical APDL (MAPDL).  This is not a problem because we can use an APDL command object to get the results from MAPDL and bring them back to ANSYS Mechanical.

## Three Simple Steps

There are three very simple steps needed to get this done:

1. Identify the geometry you want the reaction loads calculated on
Do this by selecting a face, edge, or corner and create a named component.  You will use that named component to grab the nodes that sit on the piece of geometry and do an FSUM in MAPDL. In our example, we call the named selection react_area1.
2. Tell the solver to store the required modal information
Since ANSYS Mechanical doesn’t do reaction force calculations they save disk space by not storing the info needed for such calculations, but we need them.  So add a command object in your modal analysis environment that says save all my results (outres) and expand all my modes (mxpand):
outres,all,all
mxpand,,,,yes,,yes
3. Calculate the reaction force
Now we simply need to add a command object to the post processing branch that:
• gets the PSD deflection results (set,3)
• selects the named selection (cmsel),which is a nodal component in MAPDL,
• gets the nodes attached (esln)
• calculates the reaction load (fsum)
• stores the results in parameters that we return to ANSYS Mechanical. (*get,my_).  Remember that anytime you create a MAPDL parameter in the post processor that starts with my_ it gets returned to ANSYS Mechanical. (well, that is the default, you can change the prefix)
• select everything so that MAPDL can keep post processing like normal

For our example, it looks like this:
/post1
set,3,1
cmsel,s,react_area1
esln
fsum
*get,my_fsumx,fsum,0,item,fx
*get,my_fsumy,fsum,0,item,fy
*get,my_fsumz,fsum,0,item,fz
allsel

The following figure shows the model tree for our example, and the returned parameters:

Nothing fancy, simple in fact: Make a component, store the required info in the result files, do an FSUM and bring back the results.

That was a short article!  And no exciting pictures.  So… if you want to you could check out the travels of The PADT Hat around the world.

## Ansys Elite Channel Partner

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

## Product Development

Keep up to date on what is going on at PADT by subscribing to our newsletter. Every month we share news about PADT, our partners, and our customers. We also share links to useful information on simulation, product development, and 3D Printing.  Sign up, and let's stay in touch.

By submitting this form, you are consenting to receive marketing emails from: . 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

06/17/2024

06/18/2024

06/20/2024

06/26/2024

06/27/2024

07/15/2024

07/18/2024

08/05/2024

09/09/2024

09/10/2024

10/23/2024