I will try to describe the problem first and then I'm going to ask my question.
There is a type of hydraulic throttle, which isn't functioning propertly from the certain point of increasing the volume flow.
The example picture shows the flow direction, so the piston is normally dragged to close the flow gap.
Now I'm up to check the forces on the piston to see the effect of dynamic and static pressure. I need you to show me the possibilities to
see and analyse forces on walls propertly. I'm not shure if the direction and amount of forces is correct.
My method to check if the sum force applied on the piston is "closing" was to pick all surfaces of the piston and then to look at the "forces summary".
The Result was round about 1400 N in "x" direction, but with "+", so in opening direction! Thatis why im not sure if i'm doing the right thing, so i'm not able to validate that.
Solved! Go to Solution.
I see the question must be probably complemented..
I have choosen all surfaces of the piston to analyse the forces in X-direction. The Summary shows:
As you can see the sum-force-X is "+" positive and is directed upward, but this is theoretically wrong because the piston is dragged down toward the gap.
I explain it to myself throug "the wrong side" of the surfaces i pick, because i pick them on positive side and not from within.
There are a few points to consider here.
What flow speeds are you seeing?
Is this really a compressible analysis?
Have you tried refining the mesh?
Could you share an image showing the velocity and mesh on a cut-plane through the small section?
The Analysis is incompressible and static.
The Mesh is adaptive and has 3 refinement cycles-
Further the velocity and flow-direction you can see here:
I have noticed, that in the solver-settings the option "Wall-forces" is not activated (the screenshot is showing that), sorry i have a german surface, but you can probably see what i mean.. This could probably be a mistake?
Thanks for Help
Has anyone an idea why the force is shown as positive? My next question is about the calculated force of 1500 N, is it the force which results from hydrostatic and hydrodynamic pressure?
CFD never includes hydrostatic pressure (pressure due to gravity, if you mean that). The force is calculated based on the static pressure field and the friction (viscous) field.
The reason why you see a positive force is because you have no "opposing forces" (Gegenkräfte) that may be present in reality above the piston. I assume there is some "clipping part" drawn above the piston that cuts it in two halves? Probably, if you take the whole geometry you will have a higher pressure above the piston than below so it will be pulled down.
The reason why you have such a high +X force is because you have a outlet pressure of 100 Bar gage. The appropriate way to run this analysis is to set your environement pressure to 101.01325 bar and your outlet pressure to 0 gage pressure.
Make these changes and rerun your analysis. Just run from zero and run the analysis based on the already adapted mesh. Also, you should be running these simulation to convergence. I would set at least 500 iterations to solve and not just 100.
Another tip! Define a group of surface that includes the surface that you want to use in the wall force calculator so that you don't have to individually select each surface during post-processing. If you do this after the simulation finishes just define the group and run for 0 iterations to update the post-processing.
With "static pressure" I didn't mean the P(amb) but the pressure itself which is resulted from pressure field whithin the valve like you said.
For me i see only the possibility either to take the full model of this pilotated throttle or to search the way to separate the dynamic and static forces (is it possible in Autodesk CFD?).
Anyway thak you for support