Centrifugal force on rotor blade

protontim

I have a rotor blade made from shell elements. I have specified it to rotate around the y-axis at ~500rpm. I run the simulation and the reactive forces at the anchored nodes look reasonable. I then add some lifting forces along the length of the blade. The blade appears to deflect under those lifting forces as if there are no corrective centrifugal forces acting on the blade (the centrifugal forces should act to reduce the deflection caused by the lifting forces). If I turn off the centrifugal force the deflection is virtually unchanged. How do I get the centrifugal forces to act on each element?

[Deleted User]

Have you tried a higher rpm. 500 rpm is really low. It may also depend on your blade mass. A light blade that is also stiff will not move as much as a heavy blade that is not as stiff. Try 1,200 or 1,800 rpm just to see what happens. Also try reducing the modulus of elasticity. Again, just ideas to test what is going on.

protontim

Hey prop_design,

It is a 6' radius hollow aluminum rotor. The reaction force at the "hub" is 1230lbs @552 rpm, so the centrifugal forces are significant. I bumped it up to 1000rpm resulting in a reaction force of 4034 lbs - still there is no significant difference in the lift induced displacement when I have it rotating at 0 rpm and 1000 rpm. Have you seen this compute centrifugal force on a per node basis? It looks like it is just computing it for the solid body.

[Deleted User]

I believe I did a test using shell elements once. However, for my models shell elements are not good enough to capture the geometry. So I have been using solid elements. I haven't tested how the software behaves when lift or other forces are applied. I have only been using centrifugal load by itself. Perhaps Victor will have some ideas wrt your question. I'm not sure of the differences in Mecway's shell and solid element formulations.

In the past, a long time ago, I have made shell elements of blades using MSC/Nastran as the solver. The input decks were created with custom Fortran code. Basically every element was specified so that the correct mass and material properties were applied. I have not seen any commercial software that allows you to create shell models of blades correctly. Moreover, when using off the shelf FEA pre-processors, solid elements are better at capturing the mass distribution (thus the centrifugal load). Of course, by using solid elements, you have a much larger model to solve. Now days, that really isn't an issue though.

If it isn't too much trouble, it would be interesting if you were to make a solid model of your problem and compare that to your shell model. I know in the case I did there was a huge difference. So I just went with the solid geometry from that point on.

A 6 foot radius is big, I can see why you are using 500 rpm. If your stress is about half of yield then you are probably at a high enough rpm. Not sure where you are at exactly. But using half of yield as your steady stress gives you some margin for your vibratory stress (envision a Soderberg Diagram). But comparing rpm was just a test and it seems like you aren't seeing any changes.

Another thought is the aero loads are usually very small compared to the centrifugal load, so that could also be why you aren't seeing anything change.

[Deleted User]

i ran your model and the results seem odd. The aero loads seem to be working. But the centrifugal load doesn't make sense. Not sure what is wrong but the model isn't moving in the direction you would think. It should be stretching along Z to me. I don't know if it is your boundary conditions or not. Rather than fixed boundary you have displacements set to zero. I don't know Mecway well enough to modify your model but I would try fixed boundary conditions just to be sure. Other than that maybe something isn't setup right. I can see the shell model is probably ok in your case since you are modeling a hollow blade. I was think of a solid blade. But your model the aero and the centrifugal are moving the blade in similar directions, so that is why you aren't seeing the combination of them. I turned off all the aero loads to see what the centrifugal was doing by itself. I'm assuming you have the model centered at the origin and are trying to spin it about the y-axis from what I saw.

[Deleted User]

hmm, interesting. i tried changing the boundary condition to fixed. turned out to be easy to do. the results seem to be the same. then i looked at your airfoil and see. i was thinking it's symmetrical. but it's heavy on the top compared to the bottom and heavy on the trailing edge to the leading edge. so that is probably why it is moving the way it is. surprisingly little z axis movement though. in any event, as is, the aero and centrifugal are moving the blade in pretty similar directions. i haven't run a blade shape like that before, interesting how different it moves under load. the aero loads really bend it. if you were to move the rotor so that the origin (0,0,0) was at the center of mass of the airfoil, then it should stretch along z and move more like what you want.

Victor

Since this is a linear static analysis, all forces act as if the blade is in the undeformed shape. The centrifugal force doesn't try to straighten it when it's bent by the lateral forces. You would have to do a nonlinear analysis for that. Unfortunately Mecway doesn't support the combination of features that would solve this problem conveniently. One way would be to extrude the shells to solid elements, use nonlinear analysis, and simulate centrifugal force by using gravity with several materials of different density along the radius.

As for the deflection being in a strange direction with just the centrifugal force, it seems reasonable because of the asymmetry you mentioned prop_design. I'm not entirely confident that means there must be bending though since the greater mass should be balanced by a proportionally greater tensile stiffness.

[Deleted User]

hi victor,

i'm new to mecway. i'm wondering, when i look at this file the thickness is in units of inches but the material properties are in metric units. does mecway handle mixed units. i thought everything had to be in one unit system. also, i'm not sure how to check someone else's model. for instance how could i check what units the model is actually in.

[Deleted User]

i think i figured out the measuring part. the tape measure icon doesn't seem to work in the beta version i have. but the menu item for tape measure works. so the blade is around 69in by 5 in. the material properties are in metric. just wondering if this is ok by mecway. i have been using all one unit system.

Victor

Yes, any combination of units is OK so you can just look at the units shown next to a value to see what they are for that value but others might be different. Internally, it converts everything to a consistent system for solving.

Victor

Actually, node coordinates are treated a bit differently from other values. They're displayed with whatever units the software decides you want at the time. For example if you use pounds and inches for material properties and loads, the tape measure will probably show, say 5 inches, but if you then enter a length in mm somewhere, subsequent uses of the tape measure will probably show 127 mm. I say "probably" because it decides the display units based on various factors such as what was used most recently as well as most commonly.

[Deleted User]

Hi guys,

Here are some examples to help clarify what I mean about aligning the center of mass of the blade to the axis of rotation. You can see if it is perfectly aligned you get pure tension along the z-axis (from the test.liml file). If you move the blade off to one side you get the sideways force (from the test 2.liml file). If you constrain the model at the axis of rotation and move the model off to one side you get bending in two directions (from the test 3.liml file). Test 3 is similar to the original model posted here, in that the cm is off axis in two directions and the model is fixed at the axis of rotation. Hope these help clarify the situation some.

As Victor noted, to fully see what you were originally going for, you would also have to do a nonlinear analysis. But you have to get your centrifugal load working in the correct direction first.

I cleared the results to reduce the file size. Simply re-solve to see the results, everything else is setup. I provided the step files just in case you wanted them for other purposes.

protontim

Hello Gentlemen,

Thanks for all your help. Here are a few points to clarify.

ROTATIONAL AXIS
The rotational axis is through the aerodynamic center not the center of mass. This is intentional to avoid any lift induced twisting moments. I'm okay if the centrifugal force is not exactly centered in the z axis.

ELEMENT TYPE
Shell elements were chosen for several reasons.
1) I intended to eventually simulate a composite laminate and the shell elements seemed to support this material best.
2) Trouble with accurately meshing the airfoil from a STEP file. Meshing often failed and was irregular. I ended up writing an Octave script to read in the airfoil shape data and write it to a MECWAY compatible xml file consisting of beam elements. I then extruded that shape (in MECWAY) to the required length.

INITIAL PROBLEM - CENTRIFUGAL CORRECTIVE FORCE

Victor thanks for you clarification about my need for nonlinear simulation and your suggested solution. I will look into that.

Thanks again.

[Deleted User]

looking at this more it seems like the cm of your blade is in the +x, -y quadrant. the attached model simulates closer what the resultant motion of this is. i keep thinking your model is solid. so that is why the cm is where it is, because the model is not solid.

it doesn't seem like anything is wrong with mecway or your original model. the model seems to be moving the way it should given how it's setup. if you do the nonlinear analysis, you won't get the coupling your hoping for without moving the blade cm/cg to the axis of rotation.

[Deleted User]

The biggest problem you have right now with the way it's setup is you are not getting the benefit of the centrifugal stiffening. If the blade is oriented properly the blade will stretch. This makes it much stiffer to loads in the perpendicular direction to the centrifugal stiffening. So right now your model is moving a lot from the aero loads. You should be getting so much stiffening from the centrifugal loads that it helps reduce the deflection from the aero loads. This would be evident, even in a static analysis.

Also if you view your model with thicken enabled you can see the trailing edge overlaps. This is the type of thing you can run into with shell models. Solid models prevent any kind of inadvertent errors like that. Every element is in the right place and has the right mass. That is not always the case with shell elements. But I understand about heading towards composites. Those are a whole other beast.

protontim

Hey prop_design,

Appreciate your comments. The whole purpose of this particular simulation was to explore the effects of centrifugal stiffening. It would seem to me that if the blade is undeflected in the static analysis, then the lift forces will be orthogonal to the inertial forces, hence the inertial forces will NOT provide any blade stiffening - hence the need for the non-linear simulation. Am I off base here?

I was aware the trailing edge overlapped, but it was a compromise I had determined I could live with - the mesh was generated by "hand" - actually I wrote a little script to translate the airfoil data into the xml format that could be read by MECWAY. This gave me a highly consistent mesh.

[Deleted User]

hi protontim,

that's cool that you were able to figure out how to make a shell mesh for mecway. i am new to mecway and far from being able to do that. however, the gui is doing everything i need. so i probably won't dabble in learning that stuff. i don't think the te overlap is that big of a deal, it just shows a little of what i was thinking of.

i thought differential stiffness was included in a linear static analysis. maybe i'm wrong on that. i will run some tests. victor will know the answer to that for sure. i ran a bunch of tests today. my blades are twisted so that makes it harder to see things. my blades are also solid. so a little different than your case. if you align the cg to the axis of rotation you will get more of what you want. with my blades i do get an improvement. i compared aligning along the ac vs the cg. because my blades are twisted it's a small difference but an improvement when aligned along the cg. in your case, you should see a huge difference. i haven't been adding aero loads. so i need to run some more tests, to see if the cf affects the deflection in a linear static analysis, with and without aero loads. it should. i would be surprised if you had to do a nonlinear analysis to see that, but i may be wrong. coming from ansys makes things a little confusing for me. ansys linear static can end up being nonlinear static without you really knowing it. they have kind of blurred the lines between the two, from the gui perspective. it is more explicit with mecway, which i think is a good thing.

i should mention that in all my tests, ansys and mecway give pretty much the same results. i have been comparing the two for a few months now. i have not seen any issues with mecway's capabilities. the affect of centrifugal force can get hard to understand depending on geometry. but your case seems like a helicopter rotor or rotating wing. like a guitar string, it should get a heck of a lot stiffer when cf is applied. right now, i don't think that is happening with your model.

i'm glad you posted your problem. i had been aligning my blades along the ac as well. for pretty much the same reason as you. it is more natural, coming from the aero design of the blade to think of aligning to the ac rather than the cg. but your case of a straight blade really highlights the issue. you can't really visually see the issue when the blades are twisted.

[Deleted User]

so here is some tests i did to try and answer the nonlinear vs linear question. it does seem like you have to do a nonlinear analysis, like victor said. i am surprised by this, however, i don't know the fea theory that well. the linear just seems to add the stress states more or less. when you do the nonlinear, you get the displacement reduction you expect. this is an ideal case of a symmetrical object. so the cg of the object is inline with the centrifugal force. even in your case of a blade with no twist, the airfoil is not truly symmetric. so you won't achieve ideal results. but it is still better to align the cg of the part to the spin axis. in any event, it seems like mecway does not allow shell elements in a nonlinear analysis. another oddity is that the mecway shell model is producing different results than the solid model. so it is obscuring the comparison. if you look at the case of the shell with bending force compared to the solid with bending force, that difference is throwing off the comparison some. but if you look at the solid model linear vs nonlinear, nonlinear seems to be the more accurate of the two. the test model is too big, that is why the rpm is so low. you would need to shrink the model to get the rpm up to a normal level. however, for test purposes, i don't think it matters much. once again the mecway results are virtually the same as the ansys results.

so to try and answer your original post. use solid elements in a nonlinear analysis. align the blade cg to the axis of rotation. if the blade is at an angle of attack and/or there is blade twist, the deflections due to centrifugal force is a lot different than a symmetrical object. so you need to do some tests to get your brain around it. it's hard to explain without you seeing it for yourself. but in comparisons i have done; whether the blade is at an angle of attack and/or you have blade twist, it is still better to align the cg of the blade to the axis of rotation (as opposed to the aerodynamic center or some other random point). aligning the cg to the axis of rotation maximizes the benefit of centrifugal force.

also keep in mind the soderberg diagram. you shouldn't load your part close to yield in a steady state scenario. because it will most likely fail due to vibratory stress. you need to allow for vibratory stress and steady stress. somewhere around half of yield in a steady state scenario will give you some margin for vibratory stress. that is just a starting place. every application is different. however, some people do not even think of vibratory stress. so just want to make sure you are aware of that.

lastly, composites have the same issue of failure due to vibratory stress. composite analysis is quite different than isotropic material analysis. special software is usually used. i'm not sure mecway would really be up to the task. autodesk has recently bought most of the best companies in this arena (firehole and nei nastran). so you may want to look at autodesk for composite analysis.

[Deleted User]

Here is an updated shell model. I re-did it and the results are more sensible. I was getting these same results before they shifted to the values in the previous post. Not sure what is different. Pretty weird. But the solid model would be the way to go. This is more academic than anything. Same step file was used as the previous post.

I'm curious as to why the top, middle, and bottom surfaces always report the same stress value?