The Analysis has stopped because the Solver has exited unexpectedly, RSAP>CFD

[Anonymous]

I am having a problem with running the solver of CFD 2019.

My geometric model come from Robot, wanting to have the wind traces shown for Reporting purposes. However, the solver always stops and results won't appear. It will stop without starting even the first iteration.

What seems to be the problem? I will attache the Screenshot and file here for you guys to check.

Also, it won't run on the solver at "My Computer". It will run if I make it "My Computer (Scalable)"

By the way, I am using a trial version of CFD for evaluation purposes. The File is located on my local drive. when i run the solver. 

[David.Short.]

Hi @Anonymous,

Please can you attach a [.cfz] file rather than the [.cfdst]. The [.cfz] file is similar to a zip folder and contains all the relevant files for your simulation setup. The [.cfdst] file is a stand alone file that cannot be used without the rest of the design study folder contents. A [.cfz] is created when you hit solve and can also be created by saving a 'share file' under 'save as'.

All the best,

David

[Anonymous]

---

@David.Short. wrote:

Hi @Anonymous,

Please can you attach a [.cfz] file rather than the [.cfdst]. The [.cfz] file is similar to a zip folder and contains all the relevant files for your simulation setup. The [.cfdst] file is a stand alone file that cannot be used without the rest of the design study folder contents. A [.cfz] is created when you hit solve and can also be created by saving a 'share file' under 'save as'.

All the best,

David

---

David,

Good day! here is the .cfz file you are requesting. 

I am testing out this software because we have a project which will study a smoke stack flow thru the city. I hope you can shed light.

Regards,

Jade

[David.Short.]

Hi @Anonymous,

On first inspection I would say that the external volume needs to be enlarged. Please follow this guide for wind analysis best practices.

Also your wind speed seems unrealistic (faster than category 5 hurricanes!). Using a wind speed of 10 m/s allows the model to run. 

All the best,

David

[Anonymous]

---

@David.Short. wrote:

Hi @Anonymous,

On first inspection I would say that the external volume needs to be enlarged. Please follow this guide for wind analysis best practices.

Also your wind speed seems unrealistic (faster than category 5 hurricanes!). Using a wind speed of 10 m/s allows the model to run. 

All the best,

David

---

I see, thanks for the info. I will look into it.

Regarding the wind speed, yeap that wind speed is really unrealistic but that is what is stated in the code I am using which is UFC(Unified Facilities Criteria).

I will try again and relay the results here.

edit: I am currently remodeling the external geometry volume but it crashed on me. Reported the crash with report number Autodesk - CER_181216846

edit1: I completely started again for my model. recreated the boundary conditions. with the same wind speed but different external volume size and i get this again. I thought its going to run.

[Anonymous]

@David.Short.

I still can't run the model @ 20 m/s. Does CFD have limit on its wind speed? Because the lowest wind speed in UFC is 94.72 m/s.

[David.Short.]

Hi @Anonymous,

You seem to have a number of flags applied relating to CFD2 usage but you are not solving using CFD2. With these flags removed everything seems to run fine for me. 

There is no maximum wind speed but if you apply a wind speed greater than Mach number 0.3 you will have to consider solving the the simulation as a compressible flow analysis.

All the best,

David

[bob.schlosser]

I also don't think your geometry of the table in the model is helping.  It looks like the table is made up of multiple intersecting parts.  This creates an odd mesh in the locations where the legs meet the frame for the top.  My first trial on your model with default mesh setting stopped with the same error.  When I refined the mesh it worked.

[Anonymous]

@David.Short.

Can you please identify the flags in the model? the initial model come from RSAP.

@bob.schlosser

What mesh refinement did you set?

[Anonymous]

@bob.schlosser

Actually, the model is just a test run for larger projects. That is a Cat walk just modeled as inverted. 

The model came directly from Robot

[David.Short.]

Hi @Anonymous,

Go to "Design study tools" and open the flag manager you will see three flags attached to the scenario. Remove these and you should be good to go.

[bob.schlosser]

Under the mesh diagnostic tool it will highlight edges and surfaces that CFD believes will cause issues given the current mesh settings.  I used this tool and changed the min refinement length to a value of 0.0031052.  This was completely arbitrary as I simply slide the slider over to the left until the edges didn't have an issue.  Since this model doesn't use thermal, a better solution would be to suppress the solid elements.  

The issue is that you have 64 solid parts importing from your CAD system into CFD.  This is a concern since the model doesn't appear to be that complex.  Look at the intersections of the legs and the main frame of the catwalk.  It appears that multiple parts overlapped and either Robot or CFD tried to resolve this issue by creating individual solid parts.  The mesher will force nodes along the all of the part boundaries.  I believe your model is exiting the solver during meshing because it can't mesh correctly on the extremely small parts at the center of the intersection.

[David.Short.]

Hi @Anonymous,

If you think that Bob or I have answered your questions / solved your problem please can you mark the relevant post as an accepted solution, alternatively you can allow me to mark it as such. This will help others to benefit from the discussion and easily find the solution if they have a similar issue.

All the best,

David