Variable Load Definition for pressure not working correctly

[Anonymous]

I am trying to apply a hydrostatic load in an API 650 tank and the variable load definition - linear equation base will not correctly apply the load.  The stress developed is not even close to accurate and the "linear" interpolation method gives wildly incorrect results on shells but this is identified in the help...Any help or advice?   .....  And the response I found from Autodesk about breaking up the item into parts and doing individual pressure loads is unacceptable.  

[shigeaki.k]

Hello @Anonymous,

could you try with the linear (equation based) with reference to a few points, similar to what is shown towards the bottom of the page variable load definition?

Regards,

Shigeaki K.

-----------------

If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!

[Anonymous]

I made 10 vertices on the top of the shell and ten matching vertices on the bottom of the shell and applied the load using both linear and linear eq based...both yield incorrect results. I also tried it with a single point at the center of my shell section as well as a single point at the vertices edge of the shell section...none of it was correct. Correct results were achieved using the standard method of applying the pressure load to the face and hand calculating the different pressures for different elevations. The software has the tools to not have to make this assumption and Autodesk should fix this. In a post regarding this exact issue, the official response from Autodesk was to break up the part into various sections and hand calc the various PSI and apply to the correct faces...no comment saying they would address the issue. It’s just like Apple years ago telling iPhone users they were holding the iPhone 4 wrong and messing up the signal...

[Anonymous]

I have just tried to alter the magnitude of the linear eq based load and the results give the same stress values and same deflection.  The distribution of the load is correct, seems the magnitude is not being applied or not being applied correctly.  When changing the magnitude of the linear load, the stress and deflection does change with magnitude, but as stated in my first post, this is not the correct method per the users guide.  I have attached a link to my file for review.

https://1drv.ms/f/s!Ais091ZFe2iclkAFv0BwyRRqPUIm

[shigeaki.k]

Hello @Anonymous,

thank you for the link. I have checked with the Product Team and they are aware of the issue. Unfortunately, the workaround at the moment is that suggested in the below article. I have added a note about your forum in the case raised with the Product Team.

Variable load gives wrong result in Autodesk Nastran In-CAD

Regards,

Shigeaki K.

-----------------

If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!

[Anonymous]

Has this been fixed yet? I noticed a different maybe related problem. I am applying a hydrostatic pressure to a flat rectangular plate. I tried selecting the vertices on one side to start with but the variable load definition was less focused on the other side. I tried selecting the 4 corners but then the middle was less focused. I tried creating points in the middle of two sides then then edges became less focused. Why does it not give me the option to select edges?

Also the word "scalar" is surely incorrect. Should it be "scaler" or "scale"?

[John_Holtz]

Hi @Anonymous

The variable load has not been worked on. The arrangement that I have found that works for hydrostatic loading is the following:

• flat face
• Interpolation Method = Linear equation based
• Number of points = 3 (2 does not work, no need to use more points for a load changing in one direction)

One thing that I have noticed is that you cannot type a scalar value and press the Enter key. The Enter key closes the dialog but does not "enter" the value that you type. Instead, type in the scalar value, then click another cell of the table to accept your value.

I think "Scalar" is acceptable terminology to represent the magnitude of a vector.

[Anonymous]

I will try the interpolation method - thanks for the tip. Might be worth writing up a knowledge base article to cover it until it gets fixed.

I noticed the values don't get entered but I was pressing tab which worked the same as clicking another cell.

I agree you could use scalar to represent the magnitude of a vector, however there are two ways you can look at this dialog box. You can enter the magnitude in the magnitude field (seems logical), e.g. 10 MPa, then enter a scale factor from 0 to 1 (for instance) in the "scalar" field. I have also seen it done as entering 1 in the magnitude field and entering a scale factor / scalar magnitude in the scalar field. I guess it all depends on what suits the model, but I think the former method would be more typical. And I still think scalar is misleading.

[John_Holtz]

Hi @Anonymous

Thanks for the suggestion. I just updated the article Variable load gives wrong result in Autodesk Nastran In-CAD to include the information to use the Linear Equation Based interpolation method, etc. The updated version will be uploaded to the Knowledge Network within a day or so.