Showing results for 
Search instead for 
Do you mean 
Reply
Solved! Go to solution

Displacement in FEMAP

Hi all,

 

I remember that in the past when I wanted to create an enforced displacement I had to fix the DOF in the direction of the displacement or else FEMAP would report an error.

 

Recently when I tried using the displacement type load and didnt create any constraint on the nodes or surfaces that are displaced (I created the displacement load via load on surface and also tried nodal and picked all the nodes on the surface) FEMAP didnt report any error, and the analysis results were OK.

 

What am I missing here? when is a constraint on the displaced DOF necessary and when it is not?

 

Thanks,

 

7 REPLIES
Solution
Solution
Accepted by topic author assafwei
‎08-26-2015 04:32 AM

Re: Displacement in FEMAP

Dear Assafwei,

This is not a question of FEMAP, but the FE solver you are using to solve your FE model created in FEMAP. With NX NASTRAN I can tell you that if you prescribe an ENFORCED DISPLACEMENT and do not constraint the direction (DOF) then error for sure!!. With FEMAP V11 you will see this error when writing the nastran input file of your FE model:

 

Node xx, DOF xx is not constrained but has Enforced Displacement applied.

 

Also, another explanation of why you ran without error in case of using NX NASTRAN is because the nodes where you applied the enforced displacement had as well a PERMANENT CONSTRAINT defined. Simply do a PREVIEW ANALYSIS and you will see the reason, not any trap exist.

 

With NX NASTRAN there are two methods available to you for specifying an enforced displacement at a component. The first method is to enter the value of the enforced displacement directly on an SPC entry.

The alternate method to enforce a displacement at a component is to use the SPCD Bulk Data entry. The SPCD entry is actually a force, not a constraint, but it is used in conjunction with an SPC entry to enforce the displacement. When you use an SPCD entry, internal forces are computed that are applied to the structure to produce the desired enforced displacements.

The SPCD method of enforcing a nonzero constraint is more efficient than using an SPC entry alone when you're using multiple subcases that specify different constraint conditions. Note also that when you use an SPCD entry, the displacement values entered on the SPC entry are ignored. The software only uses the SPCD values.

 

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director
IBERISA • 48004 BILBAO (SPAIN)
WEB: http://www.iberisa.com
Blog Femap-NX Nastran: http://iberisa.wordpress.com/

Re: Displacement in FEMAP

[ Edited ]

OK... now its clear...

 

I was using sol601...

Re: Displacement in FEMAP

ok!.
As Susan says "If you find my post helpful, and it answers your question, please mark it as an "Accepted Solution" -- thanks!.

Best regards,
Blas.
Blas Molero Hidalgo, Ingeniero Industrial, Director
IBERISA • 48004 BILBAO (SPAIN)
WEB: http://www.iberisa.com
Blog Femap-NX Nastran: http://iberisa.wordpress.com/

Re: Displacement in FEMAP

[ Edited ]

Done! Smiley Happy

Didnt even notice this option up untill now...

Re: Displacement in FEMAP

Hi Blas,

 

I saw this answered which is very old from 2013 but i need to understand what do you means with ''The first method is to enter the value of the enforced displacement directly on an SPC entry.''  and ''SPCD Bulk Data entry. '' . becuase i made constraint for the nodes that i export their displacemenet. It work for non-linear but when i testade to linear-nastran. It didnt work and gave me fatal massage. It seems this SPCD is the soulation but i couldnt understand it. Can you explain it to me? Thanks

 

 

Re: Displacement in FEMAP

Dear Bashar,

In FEMAP you can define an Enforced Displacement using the following steps:

 

1.- Use command "MODEL > LOAD > NODAL > DISPLACEMENT".

2.- Then you need to constraint the same DOF of the node in the same direction of the enforced displacement applied.

 

Take a look to EXAMPLE PROBLEMS no. 28 & 29 where Enforced Displacement is used (open FEMAP and go to HELP > EXAMPLES).

 

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director
IBERISA • 48004 BILBAO (SPAIN)
WEB: http://www.iberisa.com
Blog Femap-NX Nastran: http://iberisa.wordpress.com/

Re: Displacement in FEMAP

I am very happy to see you active in this group and give your experience to other people. Thanks for the answer. I have read the same answer from you also but it was in another website ( you can see it) :-)
http://www.eng-tips.com/viewthread.cfm?qid=321413

For me, it is working for the same model ( I attach a picture to explain the problem, see it below) It is working well from shell to shell. My problem is to import it to solid model. I wrote my question in the picture?