Learning Forum

[chinguanwei]

Hi all, i am doing a stress analysis on a vane component in static structural. As the vane will be rotating, i will need to apply a centrifugal force on the body. I tried locating its centre of gravity but it is not within the external surface aka located inside the body. Is there any way to do it?

I search point mass but i believe it only applies gravity force on the vane's centre of gravity. Can i tweak this force direction instead?

Thank you very much for your advise

[peteroznewman]

Static Structural has an Inertial load called Rotational Velocity.  That is what you use to create centrifugal force on the mass in the model. All you need to do is define the axis of rotation and the rotational velocity.  The solver will apply the correct acceleration as a function of the radius from the axis.

[chinguanwei]

this vane will be fitted into a rotor and the rotor will rotate. As the rotor rotates, the vane will rotate but not about a fixed point. the radius of rotation changes along the way as the rotor rotates. Is it still possible? 

May i also know how do i let this "inertial load" appear in the selection? i couldn't find it in the selection. Or is it i need to generate the point mass first?

 

[peteroznewman]

It's the third item in the list when you do a right click.  If you click on the Environment tab in the ribbon, there is an Inertial load button that has Rotational Velocity under it.

For any angle the vane can be positioned at, it is the rotor velocity that is causing a centrifugal force that puts stress on the vane.

[chinguanwei]

Regarding the point mass, what do they mean by geometry? i tried clicking on the entire selection but it doesnt select anything at all. i believe i need the point mass in order to add grabity force into my simulation?

[chinguanwei]

another problem is centifugal force is mrw*2. how do i define this radius from the CG of the vane to the CG of the rotor which it is rotatign about. 

 

 

[peteroznewman]

You don't need a point mass to add a Gravity load to the model.

You don't need to know the CG of any body in order to apply a rotational velocity load. You only need the axis of rotation.

Please reply with a sketch of the rotor and vane showing the axis of rotation of the rotor and the axis of rotation of the vane.

What is the rotational velocity of the rotor?

What is the rotational velocity of the vane?

 

[chinguanwei]

The rotor will rotates about its centre at 3000rpm. the 2 individual vanes are slotted onto the rotor. hence i am unsure of the axis of rotation of the vane.

 

[peteroznewman]

Perfect. The vanes are in translational slots and have the same rotational velocity as the rotor.

What retains the vane in the slot, preventing it from sliding all the way out and separating from the rotor?  I expect you want to model that retaining feature.

Apply the Rotational Velocity load to All Bodies in the model and specify the axis at the center of the rotor, and enter the 3000 rpm into that load.  On the Home tab, you can click the Units button and set the units to RPM.

In my model, the rotation was about the global Z axis, so I could enter the Z Component and use the coordinates of a point as 0,0,0 to define a 3000 RPM rotational velocity.  Does your rotor axis pass through the global coordinate origin?  If not, enter a point that is on the rotor axis.

[chinguanwei]

yes you are right regarding the translational and rotational. the whole component will be fitted inside a hollow cylinder.

however i am only studying the stress analysis on a single vane. the other components are not of my concern, is there anyway i can perform this analysis excluding the rotor? this is because there will be some forces acting on the area that is hidden witithin the rotor. Hence if i add in the rotor, i can't apply forces on those areas being hidden in the rotor 

[peteroznewman]

Hidden refers to visibility, but we are operating in a digital model where we are free to hide bodies that obscure our view, or section bodies to see inside.

If your primary interest is the Vane, you can apply boundary conditions to it that represent the support it gets from the slot in the rotor, without modeling the rotor. But you do want to model the part that prevent the vane from sliding all the way out of the slot. Please show an image of that feature in your reply.

[chinguanwei]

there will be a reaction force at the tip of the vane hence is not necessarily to model the part it. how can i apply the axis of rotation without modelling the rotor.  there will be pressure acting on the entire vane surface in terms of x and y axis. 

[peteroznewman]

You apply the axis of rotation of the rotor simply by entering the global coordinates of any point on that axis into the Rotational Velocity load. I showed an image of that above.

There can only be a reaction force at the tip of the vane if you add a displacement constraint.  That is what I am talking about above.

[chinguanwei]

oh ok i will try it tomorrow and let you know. thank you for the help. Sorry i misudnerstood it, ya i will be applying a zero displacement/fixed support at the tip of the vane 

[peteroznewman]

Fixed Support may be overconstraining the tip of the vane. It would be better to have a single vertex have a Y = 0 displacement constraint so that the vane is free to deform as the forces dictate.

[chinguanwei]

but in that case the simulation cant run due to not enough constraint. although the vane look like it is resting in the rotor, it is actually slanted. Hence there will be about 3-4 line support. 

In addition, do u have any shortcut on how i can find the coordinates of the rotor centre? the vane is modelled as a part file and i assembled in together with the rotor as an assembly. for the vane simulation i will be usingg the part file of the vane. 

[peteroznewman]

The vane makes contact with the faces of the slot in the rotor. That is where 5 out of 6 constraints should be delivered by Frictional Contact definitions, and only the tip constrains how far out of the slot the vane can go.

You have to use the CAD system to find the center of the rotor. You could open the geometry in SpaceClaim to do that if it is not clear from SolidWorks, but do this on a copy of the model as opening the geometry in SpaceClaim might break some of the model scoping if it was never opened in SpaceClaim before.

[chinguanwei]

everything works, thanks a lot. however I will need some advise from u. due to pressure acting on the side of the vane, the vane will be slanted rather than upright, hence not all the surfaces inside the rotor will be contacting the vane due to clearance. 

I have attached the photo here for your reference. the left vane will slant left(clockwise) with 2 line support (in green).the highest line support is due to the contact with the other vane. the 2nd lower line support is due to the contact with the rotor. Is it ok to use fixed support in this for these 2? I tried using displacement with x=0 but the constraint wasn't enough.

there will be another support at the bottom tip of the vane which is in touch with the cylinder and we discussed to keep the y component=0 

[peteroznewman]

Fixed support on two green lines is a bit of an overconstraint.

Let one green line have X and Z = 0 displacement, while the other green line has an X = 0 displacement. 

The vertex at the tip of the vane continues to have the Y = 0 displacement.

That leaves rotation about the X axis a bit underconstrained.  See if it will solve.

If it will not solve, add Z = 0 to the vertex at the tip of the vane to prevent rotation about X.

[chinguanwei]

Thanks for the help, let's say when the vane is not at the horizontal/vertical position, 

what support/displacement do you recommend me for the right vane tip? and also those earlier line support forces 

[peteroznewman]

You could include the grey body in the model as a Rigid Body. Add frictional contact between a face on the vane tip and the inner face of the grey body.  The solver will only mesh the inner face of the grey body to compute the Static Structural solution.

[chinguanwei]

so the model inside the ansys will be the grey body together with the vane? i saw frictionless support. is that what you are referring to?  

[peteroznewman]

Not frictionless support. That is what you would use when you don't have another body to make contact with.

Right click on the Connections folder and Insert a Manual Contact region. Pick the ID face of the grey body as the Target, and a tangent face on the vane as the Contact. By default, it creates a Bonded contact, so change that to Frictional or Frictionless. Frictional is better and enter a small value for the friction coefficient.

You must have first configured the parts in CAD to be tangent, which you have already done. After meshing, the discretization into nodes and elements might not put a node right at the tangency point, so you may end up with a tiny gap

Right click on the Connections folder and Insert a Contact Tool.  Right click on the Contact Tool and Evaluate Initial Contact Status. If the table shows the contact is Closed, you are all set to solve. If the table shows Near Open, you must edit the Contact to close the tiny gap.

Click on the Contact and in the Details window, near the bottom is Geometry Modification, you can set the Offset to Adjust to Touch. Now the gap will be closed.

[chinguanwei]

regarding the gravity, let's say my vane is now in a slanted position. how can I apply in the universal y direction instead of the orientation y as shown in the picture. I believe I need to create a new coordinate system but I couldn't find anything to rotate . I tried to solve the gravity force in the item x and y coorinates but then I cant type into ansys.

 

do you happen to know if there is any difference between fixed support and displacement for all 3 direction for an edge? is both the same?

 

[peteroznewman]

On a solid mesh, there are only displacement DOF on the nodes, so there is no difference between Fixed Support and a Displacement support setting all 3 directions at 0 on an edge.

Standard Earth Gravity doesn't allow you to use components.  Create a Coordinate System. If you click on the Coordinate System tab, there is a button to Rotate Z.

Now you can use that Coordinate System in the Standard Earth Gravity load.

If you want to use components, replace the Standard Earth Gravity load with an Acceleration load.  Make sure the components have a vector sum of 9.8 m/s^2. Note that the equivalent load to Standard Earth Gravity in the -Y direction, is an Acceleration in the +Y direction.

[chinguanwei]

Ok i will try it out later. Thanks for the help!

Do you happen to know if the iterative solver message pop out, does it mean my simulation is inccorrect? Or is there anyway to counter it. I am using student software. Cause if i delete 1 bc, n re add this same bc i get varying result sometime like using fixed support vs 0 displacement

[peteroznewman]

Not sure what you are talking about here.

I know that sometimes the Iterative solver will fail to converge, while the Direct solver will successfully converge.

[chinguanwei]

i cant find the rotate z axis button inside transformation. may I know how do you find that? even after I click the geometry it is still the same old screeen

 

is there any way to ensure it is direct solver instead of iterarive solver. what I meant that if I used this boundary condition like fixed displacement. I get result A, then I delete this "boundary condition" and add in the same "boundary condition" but I get result B

[peteroznewman]

When you have a Coordinate System selected in the Outline, click the Context Tab and see the Coordinate Systems ribbon. Look on the ribbon, there is a 3x3 array of small buttons in a Transform section. The top left small button is Offset X,  keep looking and you will see Rotate Z.

Click on the Analysis Settings and under Solver Type, you can select Direct.

[chinguanwei]

ok I saw the rotate z part.

For the solver type, I couldn't find the analysis setting. are you able to let me know where can I find it exactly? Thank you