Altair RISE

A program to recognize and reward our most engaged community members

Nominate Yourself Now!

Ideal Gas Compression in an Actuating Piston

Hi Good day,

I am currently working on a CFD analysis of a cylinder and piston assembly, using the AcuSolve Ideal Gas Compression in an Actuating Piston tutorial from SimLab as a reference.

Following the tutorial, I have created the fluid domain and generated a table that defines the piston motion based on a mathematical equation. I plan to apply this motion as a translational mesh motion in the simulation.

Could someone please explain the steps shown in the image above?
Specifically, under the Nodes section:

Mesh Y-Displacement
Type: Linear
Mesh Motion: Piston
Curve Fit Variable: Y Reference Coordinate
X1: 10.0 m
Y1: 1.0 m
Y2: 0.0 m

What do these terms represent? Why is X1 set to 10.0 and Y1 to 1.0?

Thanks & Regards,
Sivaprakash.

Find more posts tagged with

AcuSolve

HyperMesh CFD

SimLab

Accepted answers

acupro

The idea/intent is to control the motion of the rest of the mesh by scaling the mesh motion applied to the end face of the piston. Y-Reference-Coordinate is the y-coordinate at the start of the simulation. The moving face of the piston starts at y = 10, with the fixed base at y = 0. We want the moving face to move exactly with the defined mesh motion - so scale factor = 1, then we want the other base not to move - so scale factor = 0.

The first column is the y-reference coordinate, with the second column being the scale factor for the linear fit to the defined mesh motion. So we should have:

X1 = 10
Y1 = 1 (so at y-reference-coordinate = 10, the linear scale is 1 - move exactly with the mesh motion)
X2 = 0
Y2 = 0 (so at y-reference-coordinate = 0, the linear scale is 0 - so no motion - with linear fit in between)

From the HyperMesh CFD setup:

We need to correct the documentation to have X2 = 0, Y2 = 0.

acupro

You would use the actual reference/starting coordinates for your particular geometry. In that validation case the moving end starts at Y = 10, and the fixed end starts at Y = 0. You would use the correct locations/values for your geometry.

acupro

If the speed is constant, just set the speed. If the speed is changing - it depends on what you know.

If you know the time vs speed - use that option in the Create Table panel - and the software then determines the displacement.

If you know the time vs displacement - use that option in the Create Table panel - and the software then determines the speed.

You wouldn't specify both.

All comments

acupro

The first column is the y-reference coordinate, with the second column being the scale factor for the linear fit to the defined mesh motion. So we should have:

We need to correct the documentation to have X2 = 0, Y2 = 0.

Sivaprakash_V

Hi ,

Thanks for your reply.

I am clear why we use that option and created a table.

But I am confusing, why we assign Y coordinate as 10 .

Because, I am trying simulate the similar model and the fluid domain length is 16mm.

I assigned the rest of boundary conditions similar to the tutorial.

But I can't get the results, the mesh didn't move.

So that I am confusing about it.

Thanks & Regards,

Sivaprakash.

acupro

Sivaprakash_V

Ok, I will do the modification.

Thankyou for the great explanation!

Best Regards,

Sivaprakash.

Sivaprakash_V

Hi,

I changed the Nodal Displacement - Coordinate reference values for my geometry.
Now, It working fine.

Then in the Mesh motion, We select the face of moving body and select the direction then assign the piecewise linear curve & set speed.
In the tutorial, the speed is set as 1m/s. Is that speed matches the Time vs Displacement table.?
Else we need to manually calculate the velocity of piston then enter it?

Which one is correct?

acupro

In the tutorial it's a constant speed.

What is the motion profile in your case? Do you know speed versus time? Do you know location or displacement versus time? Etc. That will determine how to set up / define it.

Sivaprakash_V

Yes, I know the piston displacement vs time values and I have it in the format of csv.

Using the Time vs Displacement values, how to assign the speed?

acupro

I would probably leave the speed as 1.0 - then define the Time vs Displacement in that Create Table panel. Try that and see if the behavior is as you expect.

Sivaprakash_V

Ok, sure.

I will do that.

Is there any other way to assign the speed?

Or rest the speed as 1m/s and apply the respective time vs Displacement in the create table panel?

Thanks & Regards,

SivaprakashV

acupro

If the speed is constant, just set the speed. If the speed is changing - it depends on what you know.

If you know the time vs speed - use that option in the Create Table panel - and the software then determines the displacement.

If you know the time vs displacement - use that option in the Create Table panel - and the software then determines the speed.

You wouldn't specify both.

Sivaprakash_V

Ok ,Thankyou.

Best regards,

Sivaprakash.