I have the same situation as "cumulo_nimbus". my Simulation CFD solver exits unexpectedly upon reaching the "processing input" stage of the solving process. I have attached a copy of the .cfd file I was advised by the program to submit.
The context of this program is the construction of a simple 6m square house in Autodesk Revit, using generic models, which has then been loaded into Simulation CFD for a solar heating thermal analysis. I hope to understand the heating effects on the internal brick partition walls, with the sun heating the building through a north facing window and a thermally insulated ceiling preventing downward heating through the roof.
I would also be interested in obtaining further support through either basic support or advanced support, however I am a student completing this project as part of a research thesis, and as such do not have an autodesk subscription. Am i able to purchase a subscription alone, in the interest of gaining either web or phone support on a one to one basis?
I appreciate your help in this matter.
I have a few points to make on this one, here goes:
- Your main air dome is set to brick
- Your air (assuming it is allowed to move) needs to be set to Variable (right now it is Fixed so the density will be unable to change), use the lower edit option within the air material for this.
- Within materials (specifically your glass model) we have Emissivity, Transmissivity and in the background we also have Reflectivity. The sum of all 3 cannot exceed 1, right now your total is 1.92 so that will need to change. I doubt the transmissivity is really 1, that would simply have no effect on the light..
- I would just set the external dome temp to a constant value, you do not need to use transient as it is not changing
- You have flow off, is this intended?
- Assuming the air is permitted to move, you need to assign a gravity vector. I suggest 0,0,-1 is suitable here.
- The final issue is your timestep size, even with the perfectly set up model a 864s timestep will cause divergence - there is far too much going on to capture this. I would start with a few seconds at most, then stop once the flow field is more established and raise the timestep size again.
I hope that helps you move ahead.