Simulation Mechanical Forums (Read-Only)
Welcome to Autodesk’s Simulation Mechanical Forums. Share your knowledge, ask questions, and explore popular Simulation Mechanical topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Applying loads in local coordinate systems

7 REPLIES 7
Reply
Message 1 of 8
bjorn_fallqvist
714 Views, 7 Replies

Applying loads in local coordinate systems

Hello,

 

I am having problems applying a surface force in a local coordinate system. I have made a coordinate system, selected the surface nodes and set them to be active in this local coordinate system, but when I apply the load, the directions as shown (when the force is visualized) is simply shown as the directions in the global system. Is this a visual bug or something else? When I check the coordinate system axes for the surface, they show the cylindrical system I wish to apply the loads in.

 

Thanks

Björn

7 REPLIES 7
Message 2 of 8
S.LI
in reply to: bjorn_fallqvist

Personally, I believe that LCS is node-based, and has no effect on surface loads (traction/pressure).

Maybe there is a way to make LCS working with surface loads, which I dont' know.

 

So I think what you see is not a visual bug.

----------------------------------------------------------------------------------------------
If this response answers your concern, please mark it as "solved".
Message 3 of 8
bjorn_fallqvist
in reply to: S.LI

Ok, thanks. So one way to solve it would be to calculate a mean value (through the number of nodes) and apply it as nodal forces instead?

Message 4 of 8
xli
Alumni
in reply to: bjorn_fallqvist

 

Yeah, surface load as a distributed load will produce element load in analysis. It may follow element surface's orientations and its view is always global. When a Local Coordinate System (LCS) is defined with some nodes of those surface's, the generalized nodal forces are internally calculated and converted to the LCS in solving and that are not necessary shown.

 

Only do you use nodal force you have to convert it to local coordinate system if a LCS has been defined on the node.

 

-xli

 

 

Message 5 of 8
S.LI
in reply to: bjorn_fallqvist

Björn,

 

I think LCS should work with surface loads. Please test it with simple models, and let me know if there is still any issue.

Sorry for giving you wrong ideas before.

 

BTW: you are talking about MES, right?

----------------------------------------------------------------------------------------------
If this response answers your concern, please mark it as "solved".
Message 6 of 8

Bjorn,

 

Loads and constraints which support local coordinate systems (LCS) will show the LCS on the dialog when applying the load. For example, take a look at the boundary condition dialog. Those loads that do not show the LCS field do not work in a local coordinate. For example, take a look at the pressure dialog.

 

I believe the only "surface" load which supports LCS is the surface variable load (select a surface, right-click, Add > Variable Load"). For this type of load, you do not need to assign the nodes to the LCS. The dialog for the variable loads lets the user enter the equation for the variable load in any chosen LCS.

 

 



John Holtz, P.E.

Global Product Support
Autodesk, Inc.


If not provided already, be sure to indicate the version of Inventor Nastran you are using!

"The knowledge you seek is at knowledge.autodesk.com" - Confucius 😉
Message 7 of 8
benalain
in reply to: bjorn_fallqvist

An important thing has to be precised : if you remesh a model and even if you applied the lcs to surface, this associativity would not be kept

 

 

Message 8 of 8
xli
Alumni
in reply to: bjorn_fallqvist

Yes, LCS is generally referenced directly by node. So that when you remesh, node's location is generally changed so does its LCS need to be updated. Algor simulation processor will use this relationship to build global matrix in solving. So here when we talk about LCS, it always means nodal LCS.

 

Well, only exception is surface variable load that John mentioned. It allows you use a LCS as reference system, for example a cylindrical coordinate system on a piece of cylinder surface, defining the variable load function, then preprocessor will calculate the defined surface loads assembled and decompose as nodal forces. Please notice that LCS used for defining defining surface load is not applied to nodes and so that is not used in FEA calculation. There is another important fact you need to know: because this load is pre-calculated from surface and they join in MES analysis as nodal forces so that they can not be following surface deformation. Only element load can have that feature.

 

-xli

 

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report