[turbomax]

Hello,

I am trying to specify an inlet boundary condition in CFX 15.0. My inlet boundary data consists of 2D fields of P_total, T_total, and velocity directions v_z, v_r, and v_theta specified in cylindrical coordinates on an inlet plane. Since I am specifying only the velocity directions, not their magnitudes, the velocity components are for unit vectors.

My problem is that when I run the calculation, I get the following error in my output file:

ERROR #002100024 has occurred in subroutine ASS_FLX_BDINIP.

Message:
The specified flow direction on boundaries must not be tangential to the boundary. However, on the boundary patch "INLET" a specified flow direction having an angle of -4.4 degrees was found, which the solver considers as being nearly tangential.

Please do one of the following:
(1) Check your direction specification on this boundary.
(2) Set the 'Flow Direction Linearisation' to 'Velocity Magnitude' in your boundary specification.
(3) Modify the solver tolerance by decreasing the expert parameter 'tangential vector tolerance' below its default of 10 degrees.

I first tried following suggestion (1). I verified that none of my inlet velocity unit vectors are pointing in the reverse flow direction. They are not even pointing tangentially (i.e. no vectors are parallel to the inlet boundary plane).

I then tried following suggestion (3) and changed the 'tangential vector tolerance' to some lower values, all the way down to 0.0. Unfortunately this did not help.

My questions are:

1. How can I follow suggestion (2)? I cannot find anything about 'Flow Direction Linearisation' in CFX-Pre or in the ANSYS Help. What would this even do?

2. Am I interpreting the error report correctly? I understand it as saying that some of my inlet boundary velocity vectors are pointing parallel to the inlet boundary plane (or even worse in the reverse flow direction, if the angle is -4.4 degrees). Is this actually what the error report means by 'flow angle?'

Many thanks for any help or advice!

Max

[ghorrocks]

Am I interpreting the error report correctly? I understand it as saying that some of my inlet boundary velocity vectors are pointing parallel to the inlet boundary plane (or even worse in the reverse flow direction, if the angle is -4.4 degrees). Is this actually what the error report means by 'flow angle?'

I am not familiar with that error message, but it seems clear enough to me. I think your interpretation is correct.

Rather than adjusting linearisation and tolerances I would suggest looking harder to find the problem area. As you have already looked it will not be somewhere obvious. I would check around the edge of the area and where it intersects with other boundaries.

A way to do this could be to make the boundary an opening and pull some flow through. Have a look on CFD-Post and see what direction vectors it is getting at the boundary. There might be something funny going on.

[turbomax]

Hi Ghorrocks,

Thank you for your reply. I managed to solve the problem by doing as you suggested and carefully looking at the vectors at my boundary. I had previously only been looking at contours of the velocity components as I didn't realize there was a vector visualization feature. The troublesome vectors only became apparent when I visualized the vectors, and it turned out I had been using an incorrect coordinate frame. Thanks a lot!

[lxff]

hello,
I loaded the data of a calculated face into a new example through profile, and encountered the same problem as you. How did you solve it specifically？
thank you！