is there a possibilty to add additional CAD volumes/ solids into an existing CAD scene (in my case with a stl main geometry)?
Background for that question is that I want make a simulation with turning rim stars. General problem is I can only use stl file of main geometry for the reason that step file is to big for the handling in SimScale viewer (frozen browser windows).
With stl files I only have one solid but for the definition of mesh regions for MRF zones I can only pick solids. For that reason also geometry primitives does not work.
I think same problem I will get also in next step when I will try to define a porous region for radiator.
thank you very much for your answer but unfortunately that does not work.
I tried this way before I tried the way over geometry primitives.
When you convert a step-file into stl, also if you have different body volumes inside your model, you only get back one solid stl file which contains all geometries.
As I tried the way with stl faces for defining MRF zones the meshing operation stops with error messages.
In the documentation it is also written that is only possible to use volumes:
(It should be noted that to create a MRF cell zone the assigned entity should only be a ‘volume or volume set‘ and Not a face or face set. Further, please make sure that the name of the cell zone does not start with a number and does not contain spaces. For example, valid names would be “MRFZone”, “MRFZone_1”, “rotating_cells” and Not “1MRFZone”, “MRF zone”.)
You are right, until very recently the only way to create cell-zones was through the use of volumes/volume-sets.
However, a couple of weeks back, the platform was upgraded to allow the definition of cell-zones through a combination of faces as well. Please take care that the choice of faces forms a watertight (closed) body, otherwise the zone creation might not be successful.
The documentation needs an update, and is in the pipeline.
now I tried to work with faces for MRF but without success. I tried to mesh the geometry 3 times with two different geometry variants but got error messages on all operations.
In the output window in all operations it is written that generate of MRF zone will go wrong for the reason that entity mrf_rear is not watertight. But when I checked the stl model import and also at my CAD tool the geometry is watertight.
There are three issues that I wish to share with you:
Cell-zone creation: First off, your procedure of creating was spot-on, so there is nothing wrong there. The warning about one of the cell zones being open that you see in the message box is because, according to OpenFOAM’s checks, that particular geometry is not watertight. Could you try to re-create the rear cell-zone surface in a way similar to the one up front?
The First Meshing Crash: Despite one of the zones being “open”, the meshing job should ideally finish successfully - but you encountered a crash. The error shown was dgraphFold2: out of memory. This error is a known issue with the decomposition algorithm used by the meshing algorithm; it is highly non-deterministic in nature, so it is hard to give a sure-shot answer for this problem. A temporary workaround for this problem is to either (a) slightly tweak the initial number of cells in the x- y- and z- direction, or (b) change the number of processors. In your case, I tried by increasing the number of cells in all three directions by 1. This caused the error to go away.
A more permanent solution for the dgraphFold2: out of memory error is in the pipeline, and should be out soon.
Crash During Cell-zone Creation: Even though the job went past the last crash point, it then crashed during the creation of cell-zones. This error is also known, and a fix has already been developed for it and is scheduled to be released by the end of this week / beginning of next week.
Please watch this thread, I will bring you up to date as soon as it it live.
The upgrade for cell zone creation was published today - your meshing job is now successful. I downloaded and post-processed the mesh on ParaView locally. The cell zones have been created as per definition.
Here is a link to the project: SimScale Login
The name of the run is “Windkanal 4 2 mrf-fixed”.
The size of the mesh right now is 30 million cells; I would recommend using coarser refinement levels, since they would still capture the details of the geometry to a sufficient resolution of detail.
I tested the simulation yesterday night … and yes it runs with success.
Thank you very much again.
Attached a screenshot of surface velocities with vector arrows:
