[simo125]

Hello,
I'm a new user.
I've used Fluent and Ansys for three years and now I have to use Solidworks for my tests so sometimes I'm a bit confused by the new software.
For exemple:
I run the 1st calculation with a cylindrical empty body (excluded from control volume) as surface goal.
Now I would create a subdomain using this body as a lit and apply the results found on this surface as new boundary condition for a 2nd calculation.
Is it possible in solid works?
I've tried to make something similar with transferred boundary condition but the program enables me to apply them only on a rectangular domain while I would impose boundary conditions on a cylindrical subdomain.
Thanks
Greatings
Simone

[Boris_M]

Hi Simone,

I'm confused on what you generally try to do. You have to consider that SolidWorks Flow Simulation uses a cartesian mesh so the computational domain is always rectangular. It doesn't matter if you want to do a flow in a pipe or something rectagular like a desktop housing.

What is your application or test you try to do?
What are you trying to do with the cylindrical body exactly?
Use it as a pipe or a heat source or what is the goal for?
What goal are you interested in?
Are you doing a flow over a cylinder for drag?

Boris

[simo125]

Hi Boris,
I'm sorry because I've explained my problem really bad.

What is your application or test you try to do?
I'm trying to evaluate mass flow rate, pressure drops and cavitation-zones inside a gate-valve.

What are you trying to do with the cylindrical body exactly?
I run 1° "standard" calculation using the cylindrical body as a surface goal (I excluded it from Component Control in FlowSim and I choose its internal surface as goal).

Use it as a pipe or a heat source or what is the goal for? What goal are you interested in?
I use it to evaluate the parameters listed above

Are you doing a flow over a cylinder for drag?
No

Now I wolud post-process my cylinder internal surface and take the values of pressure or velocity and use them as "new" boundary conditions to apply at the same surface, which will be the new lid, for a sort of subdomain.
The reason of my question is because I would study cavitation and it requires a lot of number of cell (for my model for example I've created a 7million cell mesh) and it is too much.
So I want to create a EFD zoom (SolidWorks subdomani) but with my lids and not with transferred boundary condition.
I attach a .PNG which shows my problem in a simplest way.
The picture on the left is the first calculation (the main) and the picture on the right is how I would set my new boundary conitions (2°calculation wirh cavitation).
With the correct lids, etc... I would that the blu surface (circled in yellow) be my new inlet boundary condition surface (the outlet one is the same).
In the first calculation, this "blu" surface was a Surface Goal.
Thanks
Greatings
Simone

[Boris_M]

Ahhhh, now it makes much more sense :-)

No, it is not possible at the moment in this way as you cannot apply a distribution on a surface as an inlet condition from one to the other calculation. You still can use the zooming without it and use a local mesh at the tiny holes and you can also use adaptive refinement to refine according to the gradients in the flow.

I've never seen 7 million cells in a valve application. You must look into cavitation in pretty detail for such a small opening then.

Boris

[simo125]

Hi Boris,
ohh I'm sorry, I've pressed the wrong key.
No 7milion but 4 milion
Anyway, in the last test, for example, a travel consists in 4177 iterations with a mesh of 300k elements (about 40 hours for a travel).
Isothermal-cavitation, with the same mesh, takes 170 iterations for a travel (about 1.5 hours for a travel).
But the results are very different and (obviously) the ones which seems better are the standard cavitation.
Thanks for answer
Greatings
Simone

[Boris_M]

Hi Simone,

the reason for the longer calculation time with the standard cavitation is the full spectrum of the temperatures that are considered but if the temperature doesn't change then the caviation results should be the same and not a large difference. Are the settings in the fluid correct?

The isothermal caviation works for all fluids but was specifically designed for technical fluids such as oils, fuels etc. where usually not the full temperature spectrum cavitation properties are available in a datasheet but only certain values for fixed temperatures. Water is very well known but with the range of various different oils and other technical fluids it is very hard if not impossible to get such detailed information.

What are the pressure differences between inlet and outlet over the cavitation?

Boris

[simo125]

Hi Boris,
study fluid is water in this case and I have not heat surface or surface surce so I though that isothermal-cavitation was good.
I'm trying to find the BC that give me the cavitation triggering and the results are very different from standard to isothermal cavitation.
Tha mass flow rate should be the same after a specific delta pressure (a sort of chocking).
With the isothermal-cavitation if I increase delta Pressure, the mass flow rate decreases while with standard cavitation this not occur.
Is it possibile that SW gives me information (for isothermal-cavitation) only about the mass fraction of water inside goal and not the global mass flow rate?
Instead Standard cavitation has better result and the mass flow rate became almost the same for higher delta pressure.
In this case my pressure inlet is 24 absolute bar, pressure outlet from 3 to 0.7 absolute bar, the temperature is 362k.
Vapour pressure il 0.67558 bar.
Thank
Greating
simone

[Boris_M]

Hi Simone,

Against what do you judge the accuracy and how much is the deviation of both cavitation models against this base value you judge it against?
We did validations of the models and both are very good. Of course there are always deviations and especially with cavitation it is not easy as the bubbles can appear and burst again and therefore constantly change the flow rate and the blockage due to the bubble. So it is not always that easy.
You can find two of the validation cases in the "Technical References" PDF that should come with the software installation. We also used pumps and other cases to validate it.

Where did you get your Water parameters from?
For example there are deviations depending on which model you use to calculate them. From a table that I found I get the interpolated value of 0,67211 bar, from one equation I get the value of 0,66301 bar and from the Antoine equation I get the value of 0,67017 bar. So just as an exampe the values here vary from below 1% to 1.86%. It's not much but it might have an influence on the accuracy as well.
Have you used a global goal for minimum density? This might be important to keep the solver running until it has converged for the vapor density.
Also how much dissolved gas did you specify for both cases?

Boris

[simo125]

Hi Boris,
yes I've read Tecnical Reference and SolidWorks help before starting this kind of calculation.
About fluid, I've copied and pasted "Water Liquid" from SW Engineering Database and I used it in isothermal-cavitation, adding the other variables required (as temperature, molar mass, vapor pressure).
In this way i Thought that there were not many differences.
I used global density as goal and not minimum density and dissolved gas percentage is the same for both fluid (standard value 0.0001).
If I find the charts that I made, I'll post you the picture to explain better my doubts.
Thank for the reply
Greatings
Simone