Need help applying initial temperature to moving solid

Need help applying initial temperature to moving solid

Anonymous
Not applicable
780 Views
8 Replies
Message 1 of 9

Need help applying initial temperature to moving solid

Anonymous
Not applicable

Hello everybody,

 

I am having trouble applying Initial temperature to a moving solid. I set inital Temperatur to static 25°C to all parts (moving and non moving). When I start my simulation the non moving parts have a Temperatur as initialised of 25°C but the moving solid starts at 0°C.

So my question is, how do I set an inital temperature to a moving solid?
All help is appreciated.

 

J

0 Likes
Accepted solutions (1)
781 Views
8 Replies
Replies (8)
Message 2 of 9

Jon.Wilde
Alumni
Alumni

Are you applying to volumes (not surfaces)? Fluid as well as solids?

What else is assigned within the model?

 

Are you starting with the part outside of the model initially and using 'initial position' to move it into place? This is recommended 🙂

0 Likes
Message 3 of 9

Anonymous
Not applicable

I am applying to volumes. The initial temperature I applied to all the non moving parts are working fine. The only moving part is going through a heating shaft. Objective of this simulation is to analyze the temperature profil of the moving part in the heating shaft. My issue is that the moving part is entering the heating shaft with a temperature of 0°C even though I have set an initial temperature of 25°C.

Thanks for your help Jon

 

J

0 Likes
Message 4 of 9

Jon.Wilde
Alumni
Alumni

Not sure, sounds a bit weird 🙂

 

Could you share a support file/CFZ?

0 Likes
Message 5 of 9

Anonymous
Not applicable

Here is a simplified version of my simulation:

 

 

0 Likes
Message 6 of 9

Jon.Wilde
Alumni
Alumni

Thanks - we need a CFZ though 😉

0 Likes
Message 7 of 9

Anonymous
Not applicable

🙂

0 Likes
Message 8 of 9

Jon.Wilde
Alumni
Alumni
Accepted solution

Thanks 🙂

 

A few things:

 

  1. Start with the moving part outside of the model and use 'initial position' to move it into place - this needs a CAD change
  2. Enable 'Wall Layers' (boundary layer) before running - off by default with motion analyses and very useful to have on with heat transfer
  3. The moving part and surrounding fluid really need the same mesh. I would use a manual mesh here with a refinement region and the solid with the same mesh size
  4. You have 'auto forced convection' on. This runs flow first and thermal second and cannot be used in this type of analysis as you need both to be run together. Please turn it off 🙂
  5. I would start without radiation, get it running smoothly and then enable (usually a quicker approach to speed up testing)
  6. A 10s time step is really large considering what is happening, I would start smaller, maybe 1s or even less with something like 3 inner iterations
  7. You can set time steps to run to -1 if you like and then set a fixed stop time - easier to calculate

That ought to solve it!

 

Thanks,

Jon

0 Likes
Message 9 of 9

Anonymous
Not applicable

Hey Jon,

 

thanks a lot for your help. 

 

Best,
J

0 Likes