Discussion Groups

Simulation Mechanical and Multiphysics

Reply
Contributor
roberthaas4107
Posts: 19
Registered: ‎08-30-2012

Extracting Forces and Moments

661 Views, 5 Replies
09-20-2012 12:35 PM

If I have a model of brick elements, how can I extract the forces and moments for a cross section? I want to do this to go through calculations for welds.

 

Thanks

 

Please use plain text.
Valued Mentor
AstroJohnPE
Posts: 505
Registered: ‎08-30-2012

Re: Extracting Forces and Moments

09-20-2012 01:36 PM in reply to: roberthaas4107

Hi Robert,

 

If the welds are at boundary conditions, then it is easy to get the reaction forces from "Results Contours > Other Results > Reactions > Reaction Force (Negative)".

 

If the welds are at locations between parts, it is a little trickier. BEFORE running the analysis, you need to go to the "Solution" tab under "Setup > Model Setup > Parameters", then click the "Settings" button under Engineering Calculations. Set the "Reaction Method" by clicking the cell to set it to "Ignore" for one of the parts involved in the joint. (Because the reaction forces are equal and opposite, the net result is 0 when the calculations are done on all parts. By ignoring one of the parts, you will see the reaction forces on the mating part.)

 

Brick elements do not calculate moments. So you will need to calculate the sum of Reaction Force times distance from neutral axis. Depending on how many nodes are involved, you may want to "Results Inquire > Inquire > Current Results" and save them to a CSV file, and then use a spreadsheet to perform the calculation.

 

John Holtz, PE
Mechanical Engineer
Pittsburgh, PA

16 years experience with Simulation Mechanical
Please use plain text.
Contributor
roberthaas4107
Posts: 19
Registered: ‎08-30-2012

Re: Extracting Forces and Moments

09-21-2012 01:50 PM in reply to: AstroJohnPE

Normally the welds are located between parts. Can you explain in more depth the process of getting the reaction forces? I changed one of the parts in the file to Ignore. When I select all the nodes on a face and click "Current Results" I only see the magnitude or the force in a specific direction. Is there a way that I can get the forces in all directions into one file, as well as their locations.

 

Thanks

Please use plain text.
Valued Mentor
AstroJohnPE
Posts: 505
Registered: ‎08-30-2012

Re: Extracting Forces and Moments

09-24-2012 02:19 PM in reply to: roberthaas4107

"Results Contours > Other Results > Reactions > Reaction Force (Negative) > Vector Plot" will give all three components of the force. Then when you "Inquire Results > Inquire > Current Results" and click the "Save Values" button on the dialog, it will output all three components and the coordinates of each node.

 

Does the following make sense to everyone? Or is my logic all wrong?

However, you probably do not need to output the values, at least not to calculate the moment. The thought that occurred to me (while in the shower!) is that the engineering formulas you are presumably using to calculate the weld size based on the moment is just a formula to convert the hand-calculated moment into an axial force or stress. Since you already have the total axial force due to the axial loads and moments, you should be able to use the reaction result calculated by the software -- at least if your constraints/bonding represent the real welds. It is analogous to looking at the stress tensor for a "beam" modeled with brick elements. Those results are due to the axial stress and the bending stress that would be hand-calculated in a beam free-body-diagram.

 

Which leads to another possible way to calculate the moment should you want to. The fiber stress along the length of the "beam" equals "axial stress" + "bending stress" on the top side, and "axial stress" - "bending stress" on the bottom side. From looking at the stress tensor results on the top and bottom, you can calculate the equivalent axial and bending stresses.

 

John Holtz, PE
Mechanical Engineer
Pittsburgh, PA

16 years experience with Simulation Mechanical
Please use plain text.
Member
kimbob
Posts: 3
Registered: ‎01-13-2010

Re: Extracting Forces and Moments

09-27-2012 05:37 PM in reply to: roberthaas4107

As a side note concerning extraction of nodal forces and creating free body diagrams, sometimes I have had to split the part up into convenient pieces just to get useful nodal forces from the reactions.

 

I turned in a product improvement suggestion to present nodal forces for visible elements only.  Mathmatically this should be very easy to do, but software code for the interface might be significant work.  Autodesk contacted me and wondered why I would want this capability and I explained how usefull it is for hand calculations and sanity checks.

 

I don't expect Autodesk will do anything, at least for awhile, but I know it would be a very benificial feature for many.

Please use plain text.
Valued Mentor
AstroJohnPE
Posts: 505
Registered: ‎08-30-2012

Re: Extracting Forces and Moments

11-26-2012 05:56 PM in reply to: kimbob

In a previous reply, I wrote

 

The fiber stress along the length of the "beam" equals "axial stress" + "bending stress" on the top side, and "axial stress" - "bending stress" on the bottom side. From looking at the stress tensor results on the top and bottom, you can calculate the equivalent axial and bending stresses.

 

Because this question has been asked in a different thread, and is likely to be asked in the future, I decided to do a test model to see if the method would "work" in practice. As always in FEA, the answer is not a clear, black and white "yes" or "no". See the attached files.

John Holtz, PE
Mechanical Engineer
Pittsburgh, PA

16 years experience with Simulation Mechanical
Please use plain text.