CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (https://www.cfd-online.com/Forums/ansys-meshing/)
-   -   Creating Volume from Scratch in DesignModeler (https://www.cfd-online.com/Forums/ansys-meshing/76022-creating-volume-scratch-designmodeler.html)

Jade M May 11, 2010 14:16

Creating Volume from Scratch in DesignModeler
 
I am trying to create my fluid volume. It is relatively simple, -- 4 rectangular impeller blades in a cylindrical cavity with a shaft in the middle. I've created the geometry with extrusions and slices. I do not know whether I've actually created any volumes or if I have just created a bunch of surfaces. I've suppressed (what I think are) the volumes associated with the solid parts (impeller blades and shaft). When I go to mesh, the entire volume is meshed. It seems that in suppressing the volumes, I've only removed some of the boundaries of these solid volumes. What additional steps do I need to complete? Thanks for any information.

ghorrocks May 11, 2010 18:23

Have you done the workbench tutorials? You should know this if you have done the tutorials.

jsm May 12, 2010 06:54

Hi,

I think that you have some confusion with solid and fluid volume. The easiest procedure is

1. Make solid parts (rotor with shaft). I think that you almost done this.
2. Make another cylindrical volume around this solid parts
3. Just do boolean operation to subtract the solid parts from cylindrical volume.

Cylindrical volume is your fluid domain for the analysis.

Hope this will help U

with regards,
JSM

Jade M May 12, 2010 09:18

Thanks JSM. Your comments are very helpful. I do not have access (and I do not actually think there are any) specific to what I am trying to accomplish. I tried two ways which did not work, one of which is probably related to your comment.

For any who are interested, the following steps worked.
• Draw the shaft
Generally, the steps are to create the plane, sketch a circle, dimension the circle, and then extrude the sketch with Add Frozen. See Fig. 1 below for dimensioning.
• Draw the blades
Generally, the steps are to create the plane, sketch a circle, dimension the circle, and then extrude the sketch with Add Frozen. Note that a new plane has to be created even though this plane lies in the same plane as the shaft’s sketch. See Fig. 2 below for dimensioning.
• Create the enclosure
Create the plane, sketch the circle, dimension the circle, and extrude the sketch with Add Material
• Remove the solid parts
Click Create > Body Operation. For Type, select Cut Material. For Bodies, select the shaft and blades. For Preserve Bodies, select No.
• Split the volumes into rotating and stationary volumes
Click Tools >Freeze. For the horizontal cut parallel to the flat face of the cylinder, create a plane (offset z so that plane lies between the face and the blades) and slice. For the cylindrical cut, create a plane on one of the flat faces of the cylinder, sketch a circle, dimension the circle so that its diameter is between the trailing edge of the blades and the periphery of the cylindrical cavity, extrude the circle the full depth of the cavity. Now the volume is split into 4 volumes.
• Create the inlet
This will be accomplished by imprinting which can only be completed on unfrozen bodies. Click Tools > Unfreeze. Select the body that has the inlet surface and click Generate. Note that unfreezing all bodies will merge the bodies into one single body. Create the plane, sketch the circle, dimension the circle, and extrude the sketch. For Operation, choose Imprint Faces. To refreeze, click Tools > Freeze.
• Create the outlet
Repeat instructions for the inlet.

miyashin August 26, 2010 15:04

ANSYS DesignModeler, Surfaces -> Solid?
 
In ANSYS DesignModeler, can we create a solid (volume + surface) from several surfaces? For example, if I create 6 squares, can I create a cube using those surfaces? I was looking for something like "Solids from Surfaces" under "Concept", but apparently there is nothing like that... This must be one of the easiest things to do on ICEM CFD, but I just can't find the way to do this on DesignModeler. Of course, I'm creating more complicated geometries.


All times are GMT -4. The time now is 05:25.