December 1, 2018 at 6:41 pmhassamSubscriber
I am trying to simulate a pressure cylinder with interference fit under internal pressure and find out the stress distribution with in the cylinder layers. I have also incurred stresses due to temperature and combined it with static structural analysis. I have created a 2D axisymmetric analysis to simulate the problem. In results the internal cylinder doesn't show any pressure distribution. I am using Ansys student version 19.1. I have attached the file with this post for you to see. Would appreciate it if someone would assist me to proceed further.
December 1, 2018 at 8:58 pmpeteroznewmanSubscriber
There is a mistake in the Static Structural model for the Displacement Y=0 constraint. It is applied to 2 faces. It should be applied to 2 edges at the bottom of the screen.
There is a mistake in the Static Structural model, both parts are Steel, while in the Thermal model, the inner part is Titanium.
In the Thermal model you only have a Temperature input on one side, so the entire assembly reaches the applied temperature. Was that your intention? If so, you don't need to Solve for Temperature in an Analysis in a Thermal model, you can just Apply that Temperature as a Load in Static Structural.
When you say interference fit, I don't see any because the diameters of the two touching faces are equal.
- outer diameter of the inner part at 22 C = 28 mm
- inner diameter of the outer part at 22 C = 28 mm
You need to construct the geometry so the outer diameter of the inner part is larger than the inner diameter of the outer part to generate an interference.
Here are the values of CTE from your model's Engineering Data:
- Outer Steel CTE = 1.2E-05 /C
- Inner Titanium CTE = 9.4E-06 /C
Steel expands faster than Titanium as the temperature increases, therefore the outer part is creating a gap to the inner part as the temperature increases. Was this what you intended?
December 3, 2018 at 9:51 amhassamSubscriber
Thank you very much for your feedback
I have specified the material assignment in the structural steel model
The overlapping contact hast to be ramped (i.e. slowly increasing) to give accurate results. I will have to first get the stresses induced due to heat and in a second load step I will apply the loads (here pressures). Do you know how to go about it.
Rather than creating geometry in design phase I have specified the interference in offset as 0.136mm as shown in the picture. Will it work in the same way as creating interference fit in geometry phase ?
I have to create a heat flow with in the model. The high pressure inside the cylinder will will heat up the fluid. On the outside of cylinder there will be a heat ex-changer which will keep the temperature of the fluid in control. I have to simulate it on ansys.
Steel expands faster than Titanium as the temperature increases, therefore the outer part is creating a gap to the inner part as the temperature increases. I have tried to switch the materials but the gap is still there. My intention is only to create a functional interference fit for a cylinder with structural integrity. Materials can be changed later.
December 3, 2018 at 1:09 pmpeteroznewmanSubscriber
Offset in Contact is okay, I didn't check for that, now I understand. The offset will be ramped on over time, that is okay.
If the temperature on the outside is different to the temperature on the inside, you need two temperature BC. You only had one.
To change materials, click on the Surface in the Geometry branch of the tree. In the Details window, you have an Assignment row with a pull down. You can change the material of each surface there.
If you make those changes, do you get an interference?
December 4, 2018 at 5:32 pmhassamSubscriber
Ok I have changed boundary conditions for temperature. But even after material assignments I am still not getting a proper interference fit. The gap appears between two cylinders no matter what amount of offset i give. I am not sure if this is supposed to happen or the there is no interference fit happening in the model. I have attached the model for you to see
Thanks in advance
December 5, 2018 at 2:05 ampeteroznewmanSubscriber
No file is attached yet...
December 7, 2018 at 9:19 pmhassamSubscriber
Please check the attached file.
December 7, 2018 at 10:28 pmpeteroznewmanSubscriber
Now you have a model that works properly.
In the image above, you show a result with a Result display scale of 47. That means the deformation result is multiplied by 47 before being displayed. This causes the appearance of a gap when in fact there is no gap.
Set the Result to 1.0 (True Scale) and there will be no gap.
You can also plot the contact pressure between the two parts with the Contact Tool and look at how the contact pressure changes from Time = 1 to 2 to 3 s as the applied inside pressure changes.
If your question is answered, please click the Is Solution link below the post that answered it and click the Like link below any post that was helpful.
- The topic ‘Interference fit pressure cylinders analysis’ is closed to new replies.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- How to do the frequency response of the nonlinear vibration of a flexible PCB?
- Importing Line and Solid Bodies from SpaceClaim to Mechanical
- how to open SendCommand in Ansys
- problems facing during solution
- Still facing the same issue
- Failed to move file from solver directory to scratch directory: file.rst
- Adaptive Sizing
- Stiffness factor
- Import DAT file
- Import pressure data (coordinates and value) to ansys workbench through excel
© 2023 Copyright ANSYS, Inc. All rights reserved.