How to get a particular plane in CFD-Post?
 

Hi, all.
I want to get a circular region in CFD-Post and the equation is x^2+y^2<=1 && Z=1. I insert a plane Z=1, but this region is too big. I just want to display the circular region. How to do this ?
Thanks.

1. Insert plane.
2. Definition -> Method = XY Plane
3. Plane Bounds -> Type = Circular
4. Plane Bounds -> Radius = 1

Z is not radius but distance between coordinate system XY plane and your plane. Also note that by default plane type is "slice", so you'll see only intersection with your geometry. If you want to see full cyrcle then set plane type to "sample".

You can go to turbo mode in CFD post and intialise Rotational axis by setting axis definition then you will get Radius as variable.

With this Radius as variable you can use Surface of revolution for circular plane.

Thanks for your reply. If this circle is eccentric, this method doesn't work.

Thanks. I will try what you said.

You then may insert "User Surface" with "method" = "offset from surface", "type" = "translational" and define direction and distance. This will give you circle which center is shifted from the origin of coordinates.

You can define any shape you can define analytically by defining a variable as function of x,y and z; and then doing a user surface of a contour plot of it. For instance, if you define a variable as r = sqrt(x^2+y^2), then you can draw a contour at any radius you like and make it into a user surface. Likewise you can extend this to ellipses, parabolas or anything else you can define analytically.

This is awesome. Thank you.

ANSYS help
 

Can I select a specific Region? Can I vary the plane size? I want a very small plane at a specific location.


I have a box let say 1m x1m x10m.


I want a plane at 0.2 x 0.2 and 5m in the z axis of that box.

How is that possible?

Awaiting reply

Thanks.

You can define arbitrary shapes using limits on planes, or using contours. For instance the contour between x=1 and x=2 will be a strip 1m wide.

Help!!
 

I am having the same issue. I could not shift the plane :confused:

Could you explain further

Can you please explain. Thanks.

You are seeing the elements which lie wholly within the plane. That is why it is jagged.

CFD post plane
 

Hi Everyone
I want to measure the average temperature of the this plane (pls look st the image)

But I have a problem that I do not want to measre the boundary which are draw some lines (these are the bondaries and have very high temperature)

How can I create a plane that I can disregard the boundries and taking the average of the temperature of the plane? (May be offset the plane but of course without the boundaries)https://www.cfd-online.com/Forums/C:...\tas46\Desktop

Can I ask what is the relevance of this average temperature minus the hot bit next to the walls? Isn't the average temperature you get then going to depend strongly on how far away from the walls you let it go? Then doesn't your arbitrary definition of the surface mean that you will get an arbitrary average temperature?

A more normal variable to calculate would be the temperature rise of the fluid, from inlet to outlet. Or temperature at a certain point, or average temperature including all regions.

If you insist on calculating the average temperature minus the hot bits near the walls - you have to work out a way of defining this surface. One way would be to define a contour of temperature to define your surface. A better way would be to use the Wall Distance variable to do the contour, which should be available only if this was a SST turbulence model simulation.

Thank you very much for the answer. Actually I want to calculate the average heat transfer coeff. of this plane. So I need bulk and wall temperature. Wall temperature is the average temp of the boundaries. But to calculate the bulk temperature I thought that I should have a distance from the boundaries that makes my average bulk temperature more higher.

Do you have an idea about this? I know that CFX gives me heat transfer coeff but since it takes first node of the flow it is not logical. Also since I have no idea about bulk temperature, I could not set htc for bulk temperature (expert parameter)

The normal temperature to use the the inlet temperature as the bulk temperature. Looking at your results it would appear that your flow internal average temperature would not be far from this.