[sms1424]

Hello Guys,

I'm trying to simulate turbulent flow in duct system ( inlet is small straight duct=.5m then 90 elbow followed by long duct towards exit) as you can see in the attachment.
so far the solution does not look good at all, all curves are fluctuation heavily and energy curve keeps constant at one ( I believe that ok since no heat transfer occurs anyway?).

How can I fix my residual and get convergent? also, as you can see in the pressure profile attached, there is increase of pressure at beginning which does not make any sense!! is that due to divergent problem I m having or something else?

I have read somewhere reducing under relaxation factor could help stabilizing solution, but which one? I have under relaxation factor with velocity, pressure, and turbulent model


any input could be helpful guys.

Thanks!

[fluid23]

Well... first of all your inlet is way too close to your corner. I bet you are seeing reversed flow warnings at this inlet, no?

Second, what are your wall y+ values? Are they appropriate for your turbulence/wall model?

Third, your energy residual should not remain constant... I don't think. I have never seen this before.

Fourth, there is a good chance that the flow coming off the corner is not steady state. This would require an unsteady solver.

[sms1424]

Originally Posted by MBdonCFD

Well... first of all your inlet is way too close to your corner. I bet you are seeing reversed flow warnings at this inlet, no?

Second, what are your wall y+ values? Are they appropriate for your turbulence/wall model?

Third, your energy residual should not remain constant... I don't think. I have never seen this before.

Fourth, there is a good chance that the flow coming off the corner is not steady state. This would require an unsteady solver.

Thank you for your reply. and sorry for late response.

actually yes, I got reverse flow warning at first, but I have no control over geometry configuration because I am trying to simulate existing experimental set up.

For Y+ vales, how can I check that exactly? I used all y+ model for simulation.

I tried unsteady solver, but did not work also.

Thanks!

[fluid23]

I duplicate experimental setups all the time and have to extend inlets. You are most likely voiding your setup by not extending inlets. Do you know the flow conditions at this inlet? Is it a velocity inlet? A stagnation inlet? All you do by extending the inlet is insure that you have fully developed flow when you get to your 'real' inlet. This ensures that you are duplicating flow conditions at inlet, not necessarily the geometry beyond the inlet. Ultimately, if you know this is your inlet and it cannot extend whatsoever, you will either need to add more geometry to approximate your setup or go with field function at the inlet to get some kind of useful distribution. Flow doesn't magically appear at this location so you need to take steps to ensure it is behaving normally when it arrives at your 'real' inlet location.

For wall y+ you will want to create a scalar scene and select wall y+ as the field function and your wall boundaries as your input parts. The actual range of values you will target will be different depending on your turbulence and wall model. What are your selections for this? k-e? k-w? near wall, high wall, all wall, etc...?

When you say the unsteady solver didn't work, can you be more specific. There are a thousand reasons why it might be setup wrong...

[sms1424]

Originally Posted by MBdonCFD

I duplicate experimental setups all the time and have to extend inlets. You are most likely voiding your setup by not extending inlets. Do you know the flow conditions at this inlet? Is it a velocity inlet? A stagnation inlet? All you do by extending the inlet is insure that you have fully developed flow when you get to your 'real' inlet. This ensures that you are duplicating flow conditions at inlet, not necessarily the geometry beyond the inlet. Ultimately, if you know this is your inlet and it cannot extend whatsoever, you will either need to add more geometry to approximate your setup or go with field function at the inlet to get some kind of useful distribution. Flow doesn't magically appear at this location so you need to take steps to ensure it is behaving normally when it arrives at your 'real' inlet location.

For wall y+ you will want to create a scalar scene and select wall y+ as the field function and your wall boundaries as your input parts. The actual range of values you will target will be different depending on your turbulence and wall model. What are your selections for this? k-e? k-w? near wall, high wall, all wall, etc...?

When you say the unsteady solver didn't work, can you be more specific. There are a thousand reasons why it might be setup wrong...

It's velocity inlet, the thing is I am trying to simulate where the flow becomes fully developed in the horizontal duct downstream the elbow, do I have to care whether I have fully developed flow at inlet in this case?

For turbulent model, I am using K-w model with all wall model.

Thank you so much!

[fluid23]

Help me understand your experimental setup. How does air arrive at your inlet? Is it pulled from ambient conditions and open to the ambient air?

k-w is a good choice for separated flow. For all wall y+ you want to keep your y+ values between 1 and 5 or 30 and 60, but you can live with 5-30 but with some loss of accuracy. For best results k-w should be used with near wall model and y+ kept to around 1 or less, especially for separation/re-attachment purposes.

[fluid23]

For what it's worth, I suspect that you are looking for re-attachment and re-development after the corner. This will be somewhat affected by your inlet conditions, but I can assure you that just having a velocity inlet in the location you show is a bad idea.

[sms1424]

Originally Posted by MBdonCFD

Help me understand your experimental setup. How does air arrive at your inlet? Is it pulled from ambient conditions and open to the ambient air?

k-w is a good choice for separated flow. For all wall y+ you want to keep your y+ values between 1 and 5 or 30 and 60, but you can live with 5-30 but with some loss of accuracy. For best results k-w should be used with near wall model and y+ kept to around 1 or less, especially for separation/re-attachment purposes.

It's HVAC problem,Flow discharge from air handling unit (AHU) with V=3m/s and pressure=62 pa.then entered to small vertical duct followed by elbow and then to horizontal duct.

I am trying to simulate velocity profile and pressure profile to see where fully developed flow occurs along the horizontal duct.

[fluid23]

It sounds to me like you want a fully developed turbulent profile. I definitely would recommend extending the inlet at roughly 5 hydraulic diameters (maybe more) upstream to allow for this to develop.

You shouldn't have to change geometry, just use the extruder mesher. Refer to help manual for details...

[sms1424]

Originally Posted by MBdonCFD

It sounds to me like you want a fully developed turbulent profile. I definitely would recommend extending the inlet at roughly 5 hydraulic diameters (maybe more) upstream to allow for this to develop.

You shouldn't have to change geometry, just use the extruder mesher. Refer to help manual for details...

I will try to do that, and see how it goes.

Thank you for your great help!