## General Mechanical

Topics relate to Mechanical Enterprise, Motion, Additive Print and more

#### Load combination and apply pressure

• thanhttdt
Subscriber

Hi everyone,

I have a question that

1.      How to set up these loads combination in Ansys workbench in 1 block (figure a) or 2 block (figure b)

2.      How to apply pressure load in random position on the plate instead of split surface (I just see remote force, but no remote pressure)?

For example: there is a platform (figure 1)

Figure 1: Geometry topology of platform

·        Load combination 1: Pallet lifter weight

This is an attached file: https://drive.google.com/drive/folders/1kQqVOflaKY1rz2i6v37YWUn829UW48aI?usp=sharing

Best Regards,

• Sandeep Medikonda
Ansys Employee

Hello thanhttdt,

In order to create a coupled analysis, you just need to drag one analysis system onto the other.

so for a figure a, drag and drop the geometry from the Component systems on the left-hand side of workbench project page and then drop a Static structural Analysis system onto it. Follow the same procedure for figure b as well where you can drag another Static structural analysis onto the Model cell.

Check out the thermal-structural analysis set up here:

Regards,

Sandeep Medikonda

• Sandeep Medikonda
Ansys Employee

Also, I don't quite follow the second part of your question.

It is my understanding that when you apply a Remote Force, it is equivalent to a regular force load on a face or a force load on an edge, plus some moment.

Now, pressure is a scalar, typically applied perpendicular to the face. So, you can create named selections in your model and apply pressure to those faces.

• thanhttdt
Subscriber

So it means that if I want to apply pressure on the plate, I have to split this plate into some smaller pieces first and then apply pressure on these small items, is it right?

And there is no way to apply pressure on the random placed on the plate without splitting.

Is my understand true?

Thanks for kind help,

• peteroznewman
Subscriber

Hi thanhttdt,

I created a named selection using the Worksheet option to select Element Faces within a range of X and Y coordinates as shown below.

However, when I tried to use that Named Selection in a Pressure, it wouldn't take it. I wonder if someone knows why.

I also tried to make a Named Selection of Nodes, and couldn't get that to show up in a Force assignment either.

I was using ANSYS 18.2.   What version are you using?

Best regards,

Peter

• thanhttdt
Subscriber

I use Ansys 18.2 too

Would you mind to suggest me some solutions

Now I have to check vehicle tyre print pressure. So there are some position of tyre print need to be checked.

If I split the top plate, it seems unreasonable

• thanhttdt
Subscriber

Did you get this situation?

But if I select a plate, I can apply pressure there

If I only select a group of element, same story with you happen, cannot apply pressure with this selection.

It's a bit confusing here

• peteroznewman
Subscriber

Hi thanhttdt,

I checked the ANSYS Help file and the entry for Force under the category of Topology, Nodes are supported, while the entry for Pressure under the category of Topology, there is no mention of element faces (I didn't expect nodes since pressure needs an area). I should put this in as an enhancement request, since you have a good example of why it would be useful.

I'm curious why, when I had a worksheet that selected nodes, I couldn't apply a force either, just like you saw for pressure. This should work and I hope someone can explain why it's not working.

If this was to work, you could convert the pressure to force since you are selecting an area.

I have attached the ANSYS 18.2 archive.

• thanhttdt
Subscriber

Let me explore it and hope that somebody else can help

• Aniket
Ansys Employee

Hi thanhttdt,

I haven't checked entire thread carefully, but if you have a nodal named selection as shown in one of your replies above you should be able to use nodal pressure. Nodal pressure can only be applied to a nodal named selection, for some more information please check

Ansys Documentation>Mechanical Applications>Mechanical User's Guide> Setting Up Boundary Conditions>Types of Boundary Condition>Direct FE Type Boundary Conditions>Nodal Pressure

I hope that helps!

• peteroznewman
Subscriber

Thanks Aniket,

I see it now!  I almost never apply loads direct to nodes but thanhttdt has a good application for it.

You can now easily edit the Upper and Lower Bound values to move the pressure around.

The next improvement would be if you can have those Upper and Lower Bound values be parameters!

Best regards,

Peter

• thanhttdt
Subscriber

Hi Aniket,

However, let me ask you that do I use Node force or Node pressure for Selected nodes?

As you said "The next improvement would be if you can have those Upper and Lower Bound values be parameters"

It means that I can use parameter to change the tyre-print easily, right?

Now, I'm looking for new approach by using APDL code in workbench to choose Name selection and apply Node force. However, it's a little bit hard for me right now, so if you have any ideas, please give me some advice.

Many thanks

Best Regards,

• Ashish Kumar
Forum Moderator

You may apply the nodal force/ pressure in following way:

1. Create named selection. This creates a nodal component of the nodes in the input file for solver, same as creating a nodal component via CM command.

2. Insert a Commands object under the setup and define the commands:

==============================================

CMSEL for selecting the nodes defined via named selection

F command to apply force

SF command for pressure on nodes

ALLSEL,ALL !Select Everything

===============================================