Cancel
Showing results for 
Search instead for 
Did you mean: 

Documentation

Creator
Creator

Hi,

 

I am printing out the SPC forces by:

List > Output > Results to Data Table > Nodal > Total SPC Forces

 

I know these loads are the ones going from the support to the node but my client is asking for a technical document that states this clearly. I could not find any useful information in the FEMAP "commands.pdf" or FEMAP "User Guide" documents.

 

Any hint would be highly appreciated.

9 REPLIES

Re: Documentation

Siemens Phenom Siemens Phenom
Siemens Phenom

I'm not sure if I am understanding your question correctly, but the Total SPC force is the Femap vector 51..Total Constraint Force. 

Re: Documentation

Creator
Creator

Thanks @RCatania. I am looking for a document (hopefully from Siemens) the explains what this vector is and how it is formed from the output file. Does that make sense?

Re: Documentation

Valued Contributor
Valued Contributor

You may be able to demonstrate where forces are coming using grid-point force balance.  It'll tell you the

source of the forces (element, applied, reaction, etc.) and give you the total.

 

You'll need to check the "Force Balance" flag in the Analysis "NASTRAN Output Request" to get them, but the results look like this (message window):

 GPFB.png

 

 

"F-OF-SPC" is a boundary condition.  If you see "F-OF-MPC" it's a rigid element

 

Totals should be zero; this is effectively a free body diagram on the node.

 

Then confirm the output vectors via query:

Query.png

 

 

 Totals are the resolved components.  In this case, I've got a T--zR--- constraint so total = T3

 

 

 

 

Re: Documentation

Pioneer
Pioneer
Ewiener,
He is looking into the document, which talks about the SPC forces (Reaction).
When Analyzing simple cantilever beam, you are fixing the one of the support and applying load at the free end.
And we look for the SPC forces at the fixed end. These SPC forces are nothing but Reactions which acts from Ground to the cantilever beam.
But to look into the forces that the structure exerts on the wall, we need to change the direction of the reactions to get the same force
is that correct..?

Re: Documentation

Creator
Creator

Thanks @EWiener! I see your point. However, please take a look at what I get from my Force Balance request:

 

FB.PNG

 

 

 

 

 

 

 

I am using NEiNastran. The numbers are correct for the Elem1 and Constraint, however, I cannot make sense of the **Total**. Why is it negative? To avoid this sort of confusion I am asked to provide evidences from the software manual to explain what exactly each type of the loads we print out are.

 

PS: in simple models it is easy to verify the direction of the SPC forces. But in our case, we are dealing with a rather complex model of a rack attached to the structure of an aircraft. Aircraft structure is not modelled. The rack, instead, is constrained through SPCs at its interface points. We need to show the SPC forces that we print out from the model are the loads which are applied to the rack not the reactions that are applied to the aircraft structure.

Re: Documentation

Valued Contributor
Valued Contributor

Ok...thanks for that screenshot

 

Negative numbers are possible in the sums (it's the vector direction) so I think that concern is minor. 

 

The major one is why your total is not zero (or nearly e.g. -7.8046760 E-10). 

 

If you are doing a GPFB on a constraint, the reaction force shows up as "F-OF-SPC", but again, the total should be zero.

 

If you're using contact regions, you can get F > 0, but you'll see it and can confirm via the "query" command:

 

GPFB + Query, Glued.png

 

I'm suspicous why the force total is exactly 1 (lbf or N).  Usually when I get "exact" values it's a clue something isn't quite working.

 

You may need to do some debugging to find out what's going on.  

  

I also need some help understanding "SPC forces we print = loads applied to rack, not reactions applied to A/P".  If your boundary is the rack <-> A/P interface, that's where your free body diagram section cut.

 

So if you're standing on the Rack and apply +1g Z, the reaction is down.  When you "step onto the A/P", the loads are equal and opposite; they're applied to the A/P as +1g Z

 

Rack  - AP FBD.png

 

Maybe you just need to dump the SPC/Reaction loads into excel and multiply by -1?

Re: Documentation

Creator
Creator

Thanks so much @EWiener for taking the time and discussing this further.

 

I think the reason **Total** isn't zero is that I am doing the GPFB at a SPC-ed node. When I repeat the same process for an internal node the total is near zero, as we expect. Thing is I am not sure if this TOTAL is the same as the SUM. I wish I could find a document that explains what each of these are.

 

Your analyses and free body diagram of the A/P is perfect and I am in line with it. The way our problem is modeled is shown below. The parts in blue are not modeled and are shown here only for clarity. The green part is modeled and loaded and constrained as shown.

pp.PNG

 

Since it is statically indetermine, we need to show when we are reporting the SPC loads from FEMAP, these are the loads that are acted to equipment (shown in green) from the A/P, not other way around (from equipment to the A/P). We think the best evidence could be a document which states this clearly. Unfortunately, I haven't seen any yet.

 

Re: Documentation

Valued Contributor
Valued Contributor

I think something is still going on thou...When you do a GPFB at a constraint / SPC you should get a line that says "F-OF-SPC". 

 

Reference my first posting and the GPFB.  "F-OF-SPC" Fz = +74350.875. 

 

That the the Reaction force on my FE model that is counteracting the -16.095587 applied load and -74334.7734 in element 74333.

 

Here's the FBD, with the matching "reaction" force from the SPC/Constraint.  The vector is UP matching a +Z notation.

 

Reaction at BC (T--zR---).png

 

 

"F-OF-SPC" = Constraint Reaction Force = Force acting on my FEA model.

Re: Documentation

Valued Contributor
Valued Contributor

Reactions on your FEA model must be equal and opposite to the forces applied to the A/P; that's the fundamental of a FBD.

 

However, if as you state the Part ↔ A/P interface is indeterminate, you must model the A/P.  The load distribution is dependent on the stiffness of your part and the stiffness of the A/P.  

 

If you don't model the A/P and your Part boundary condition = a SPC you're stating the A/P is infinitely rigid.

Part - AP.png