## General Mechanical

#### Localised pressure from compression ridges

• akman88
Subscriber

Hi Ansys community,

Please bear with me as this is my first post and I am novice ansys user.

I am trying to simulate a localised pressure around extruded ridges. The whole structure can be seen below.

The extrusion of the compression ridges can be viewed on these images below.

I have placed a frictionless support as this 1/4 of the structure with repeated profiles around a circle . From my understanding, the frictionless support could be used to provide symmetery. One fixed support was placed in the edge of the part as a boundary condition.

The force are being placed on the structure with a 1400N preload from the two bolts

My question is, when I solve the simulation, intuitively,  I was expecting the ridges from the beige to exert a localised pressure on the part underneath it. However from my result, it showed that only the deformation from the bolts instead seing a localised deformation on the part underneath the beige part from the ridges. I hope that makes sense.

Can anyone help me to explain the result of my simulation?

Did I set it up wrongly?

Why am I not seeing the pressure from the ridges?

Thanks a lot for your time.

• peteroznewman
Subscriber

No images are showing. Please edit your post and use the Insert Image button to select an image file stored on your computer.

• akman88
Subscriber

Hi Peter,

Thanks for the advice. I have edited and updated the images.

• peteroznewman
Subscriber

You ignored the Warning...

You must reduce the element size on the thin plate to get at least 2 elements through the thickness of that plate.

Don't use Frictionless Support on the ridges. That creates a frictionless contact with an invisible copy of those surfaces that are grounded. Delete the Frictionless Support

Use Frictional Contact between the ridges and the opposite face that they press against.

• akman88
Subscriber

Hi Peter,

Thank you for your advice. I managed to solve the simulation with increased deformation across the surface. I reduced the element by having a body sizing with element of 0.25mm. It is very small which increased computational time to 3 hours to solve the simulation. The ridges are very small with a thickness of 0.3mm and width of 0.5mm.I tried face meshing on the rdiges to have small element just on the ridges, but the solver could not mesh it properly. See image below on the final mesh. By any chance do you know a workaround where I can have small meshing just on the ridges instead of the whole part?

1)

2)

For the contact setting, I changed the contact to frictional contact between the ridges and the opposite face they press against. I kept the frictionless support on the side and one edge as a fixed support. See images 3 and 4.

3) Frictionless support

4) Fixed support

The result are seen as below

5) Deformation on part with ridges.

6) Deformation on part on the oppositre face that the ridges press against.

Do you know why I dont see the ridges being planted on the opposite face that they press against. Im trying to design the ridges to press against an elastomer (Viton) to provide fluidic sealing. My objective is to know how much pressure that the ridges exerted with different bolt preload. See image 7

7) What I expected to see on the opposite face that the ridges press against in red drawing (excuse my poor drawing).

It will be great if you could help me to understand this result, please.

• peteroznewman
Subscriber

Insert a Contact Tool into the Solution Branch.

Insert a Pressure result into the Contact Tool

Look at the Pressure plot.

• akman88
Subscriber

Amazing! It works!

Thank you for your time and knowledge sharing!

• akman88
Subscriber

Hi Peter,

I have a follow up question - The pressure are higher near the bolt and less away from the bolt, which is expected. I am trying to figure out why most of the ridges actually have zero pressure? Any input would be great.