Stuck? 
support@mecway.com
support@mecway.com
Mecway
FEA
Modeling gears and contact
Hello Victor,
I ask for advice for modeling the rotation of the following system. A moment is applied to the shaft, so that the shaft makes the circular-segments-plates to rotate. The gear contact is being the difficult issue to be modeled. After looking in the manual and in the forum, I found the tools of combining beam elements with solids; constraint equations; contact (CCX). At the moment, I obtained no results. I still remain with the following doubts:
1. First, I wanted to use the Constraint equation of internal solver. Using the relation between the gears, I applied on a node of the circular plante and on a node of the shaft: [rotation in the shaft] = [13 x rotation in the plate]. It did not work. I guess that the reason is that "node rotation" constraints cannot be used on solid elements, but on beam or shell elements.
Could I bond a beam element to the shaft and another beam to the plate, in order to apply that constraint equation? Or should I use shell elements for all the bodies to be able to apply rotation constraints?
Must I model the real teeth and apply to them the Contact of CCX?
2. Before modeling the two supporting rolls, I modeled the round surface of the plate as a frictionless support. Can frictionless support model the cylindrical sliding? Must the mesh be fine enough? I have this doubt because mesh elements have plane surfaces, whith theoretically cannot rotate.
3. I tried to simulate in the same model the shaft and the 8 plates to measure the twist of the shaft and of the plates. Once I obtain results, how can I measure the rotation in solid elements? Must I calculate them manually from the displacements?
Thanks
I ask for advice for modeling the rotation of the following system. A moment is applied to the shaft, so that the shaft makes the circular-segments-plates to rotate. The gear contact is being the difficult issue to be modeled. After looking in the manual and in the forum, I found the tools of combining beam elements with solids; constraint equations; contact (CCX). At the moment, I obtained no results. I still remain with the following doubts:
1. First, I wanted to use the Constraint equation of internal solver. Using the relation between the gears, I applied on a node of the circular plante and on a node of the shaft: [rotation in the shaft] = [13 x rotation in the plate]. It did not work. I guess that the reason is that "node rotation" constraints cannot be used on solid elements, but on beam or shell elements.
Could I bond a beam element to the shaft and another beam to the plate, in order to apply that constraint equation? Or should I use shell elements for all the bodies to be able to apply rotation constraints?
Must I model the real teeth and apply to them the Contact of CCX?
2. Before modeling the two supporting rolls, I modeled the round surface of the plate as a frictionless support. Can frictionless support model the cylindrical sliding? Must the mesh be fine enough? I have this doubt because mesh elements have plane surfaces, whith theoretically cannot rotate.
3. I tried to simulate in the same model the shaft and the 8 plates to measure the twist of the shaft and of the plates. Once I obtain results, how can I measure the rotation in solid elements? Must I calculate them manually from the displacements?
Thanks
Howdy, Stranger!
It looks like you're new here. If you want to get involved, click one of these buttons!
Comments
2. Yes, you can use frictionless support on a circular surface and yes there can be some binding caused by an irregular surface, but it's not as bad as the faces of a bolt head being gripped by a spanner. At each node, it uses the direction of the average face normal of the faces sharing that node, so if the mesh is uniform and a complete circle, then it'll be completely free to rotate. If the mesh is linear elements and nonuniform, or at the ends of the arc, there may be some spurious binding. However, if you use quadratic elements with their midside nodes along the circular arc, then it'll be so close to circular that the small error usually doesn't matter.
Alternatively, use an ordinary displacement constraint with a formula to make the direction perfectly radial.
3. You can connect a soft beam or shell to the solids at the point you want to measure, or create a formula in the solution that calculates rotation angle from displacements and positions. That would show angles for the whole model all at once.
1. Finally I was able to couple the rotation through beam elements.
2. Ok. I had no problems with that cylindrical sliding.
3. I only have still a question on this issue. Is the formula addressed to each node and using parameters of each node? If the center of rotation is displaced, I will need the coordinates of the displacement of the center of rotation (or another point) to calculate the rotation in any other point, right? I mean to calculate the angle by this formula. The dot product couples parameters of two or three nodes.
I don't completely understand what you mean by the center of rotation being displaced. If you know the center of rotation then you can use that in the dot product formula to find rotation angle of all nodes about that point. If you don't know it or it's twisting in a complicated way, then I don't know how would you calculate that.
For the easier case of rotation angle about the global origin:
θ = acos(r·(r+u) / (|r| |r+u|))
The formula tool only uses scalars, so you have to expand the dot product components like this for angle in 3D:
acos( (x*(x+u.x) + y*(y+u.y) + z*(z+u.z)) / ( sqrt(x^2+y^2+z^2) * sqrt((x+u.x)^2 + (y+u.y)^2 + (z+u.z)^2) ) )
or, for angle about Z
acos( (x*(x+u.x) + y*(y+u.y)) / ( sqrt(x^2+y^2) * sqrt((x+u.x)^2 + (y+u.y)^2) ) )
From your answer, I deduce that a manual calculation is needed for calculating theta.
Sorry if it looked like I was explaining basic maths. I wrote out those formulas in Mecway's formula format so you can copy and paste them in to get a feel for its capabilities with minimum frustration.
I have been following your interesting post.
I have only been able to force rotation by beam elements or as a displacement imposed on elements at the same distance from a certain origin. Each one has their disadvantages from my point of view . See attached examples.
I can’t figure how did you manage to couple different element rotations through coupling using the dot product formula.
I can introduce a displacement on each node depending on the pseudo time but nor depending on node position (it tuns red as shown in picture).
¿How could I force the same angle rotation to all geometry nodes or a displacement constrain depending on its distance to the center of rotation?
¿Could you please post a simple example file.? A plate with a few elements or similar.
Thanks for the help.
It doesn't let you specify the displacement amount as a formula in terms of position. Do you really want to leave them free to move radially and axially as opposed to locking them all together with a rigid body and rotating that?
"I can’t figure how did you manage to couple different element rotations through coupling using the dot product formula"
As Victor replied, the dot product-formula was intended to measure rotation, not to impose rotation. In this respect, I have written that a "manual calculation" is needed. However, later I thougth that the easiest solution lies in the first Victor's answer: using beam (or shell) elements to measure. I think in attaching a beam to the element to be measured --> coupling the rotation of that beam to the rotation in another beam which is aligned with global X, Y or Z --> reading the rotation that is shown in this beam, for which not additional formula must be entered.
"¿How could I force the same angle rotation to all geometry nodes or a displacement constrain depending on its distance to the center of rotation?
¿Could you please post a simple example file.? A plate with a few elements or similar."
I this file I applied what I wrote above. I give beams a higher stiffness than the plate. Mathematically it looks right: I prescribe 90° rotation and I measure 90° in another part of the body. The only thing I do not understand is the Deformed view: it does not rotate 90°.
Since it's linear analysis, rotation angles should be small to satisfy linear approximations like tan(θ)=θ. That's why it doesn't rotate properly at 90 degrees.
Mecway doesn't have a direct way to prescribe the rotation of a whole set of nodes about a single axis. However, if you don't mind also constraining them radially, you can do it using bonded contact. Here's an example that makes the whole surface rigid. You could also use a softer material so the surface can deform in all directions or probably an orthotropic material to constrain them only in the tangential directions if you really wanted that.
I,m working on the validation but meanwhile, numbers seem reasonable.
Gears are fully shells so I think I will manage to get a <1000 nodes file to share.
<img src="https://mecway.com/forum/uploads/editor/6q/e230wx6gajk4.png" alt="" />
This is how I have engaged the two gears.
Mesh is very raw and model is not completed to keep it below 1000 nodes but it contains all the elements to show how I would do the set up. It runs in 30 sec.
Notes.
This is the nonlinear option where both gears can indefinitely rotate. (Solution where output gear is attached to a rotational spring is not considered and can be found in youtube)
Rigid body don’t work properly with shells, so it is applied to a solid ring merged to the inner circle of the gear.
Input gear movement is induced with a rotation BC applied to the REF node.
I have tested tree different ways to engage the gears.
1- Brake. Easiest for me and shown in the file.
2- Traction on output rigid ring. Very hard to make it converge and only for small rotations.
3- Moment on output ref node. Didn’t manage to make it work.
Please comment if you have any idea or suggestion to make it in a better way. I still must finish validation.
Note: If any one wants to reproduce the full model by it’s own, Spur gears have been generated in a very cool webpage that generates you the dwg file for free.
Deviation from expected maximum tooth-root stress σFP is 1.4%.
Check has been done according ( ISO 6336-3) and the help of a free access online calculator.
Details on the pdf. I have measured the tangential force that the brake imposes on the gear (friction force) and measured the corresponding Maximum stress on the root for that tangential force. All safety and load factors =1 as we are validating not designing.
I'm doing it in 3D because my gears are not completely uniform in cross-section, since I have seen some 3-dimensionality that increases the stresses on the center of the gears and since I am partially interested in knowing the line-load to calculate face load factors to compare with iso 6336.
Because I'm mostly concerned with the bending stresses, I move my gears to the highest point of single-tooth contact in the CAD program (solidworks) by applying a contact constraint between the tip and flank of the gear pair that is either leaving or entering contact next. Only the tooth being analyzed and its closest neighbors are modeled to conserve elements in the mesh.
In Mecway, I mesh with a fine mesh density on the contacting flanks and a slightly coarser mesh in the root fillets and non-contacting flanks of the meshing teeth.
The tooth contact is made as a frictional contact, one gear has a fixed support at its center circular surface where it would connect to a shaft with splines and the other gear has a frictionless support on a cylindrical shaft that is modeled as one piece with the gear. The driving gear is also given a low-stiffness elastic support along the perimeter to aid stability when contact is being initialized and it is given an axial displacement constraint and a moment onto the shaft.
I had some issues which Victor helped me resolve, which was that the frictionless support on the shaft could react a moment if the elements were meshed without midnode on surface as the mesh would then be polygonal. Mecway uses the normal directions of the mesh to define frictionless supports while I had previously been used to Ansys which uses the geometry faces to define the normal direction so it is mesh independent. The issue was observed in part by doing a surface integral of the contact pressure and comparing it to the analytically calcualted forces from the gear mesh.
To calculate the face load factor, it was really cool that the nodal coordinates of the flank and contact pressure was easily exported by clicking the "new table" button next to the deformed view buttons. It let me easily make a line load by summing up the pressure in different sections of the tooth and dividing by the tooth height. The calculated line load seen on the graph below was pretty irregular and mesh dependent because of the irregular mesh with the automatic meshing compared to what I had seen previously when using Ansys which could make a very regular mesh on the flanks using "mapped face meshing". Because of this, the mesh density on the face would need to be much finer if this method is to be used. Nonetheless, the concentration caused by edge contact is very visible and shows the nescessity of either adding crowning, end modifications or something similar to gears to get an even and constant line load.
@disla , I see that you read out the von mises stress in the tooth root and compare to the values from ISO 6336 but this is not correct since ISO 6336 estimates the principal stress and not the Von Mises stress. Also, the fillet geometry may be incorrect if the webpage you downloaded the geometry from wasn't very careful in their modeling, since generated gears have a trochoidal fillet and not a circular fillet which is much easier to draw. If the fillet geometry is incorrect, then of course the calculated stresses will be too.
Last but not least, I see that the online strength calculator states a contact ratio factor which is a bit controversial by the way it increases the allowable force by assuming that some load is shared between teeth but since the contact ratio is less than 2, there are some time where only one tooth is in contact and this is why loading at the highest point of single-tooth contact is important. Contact ratio factor currently isn't included in ISO 6336.
I would like to extensively comment and ask you, but I don’t want to abuse nor boring the users which I suppose are mostly interested on the practical aspects than the ISO or theory itself.
Also, consider that this is not my area at all, and the model pretended to be an example on how to approach an assembly of moving elements and their contact.
If you agree, I would like to do some questions/comments. I will understand if you don’t want to give more details.
1-Regarding the engaging, my first approach to solve the system was the same as yours, Output gear fixed, input gear Moment, but I quickly realized something that maybe you could respond.
¿How do you know that the maximum Stress is at your gear’s positions, and even more, how do you know that the maximum contact and bending stress, arise simultaneously?
That was the main reason why I decided to certainly complicate with brakes and find a way to engage both gears free so I could inspect the whole contact path.
2-I think that the 3-dimensionality increase in the center of the gears could be in part since Shear Stress in Shells is constant through thickness in the actual formulation. So, I also agree 3D should be the most accurate approach if we are interested in the contact area. Victor is improving the shells formulation in this sense.
3-I was also mainly interested in the maximum bending Stress in the root, and I didn’t pay “as much” attention to the contact area as you. I supposed that resultant stresses far from there didn’t care about contact penetration, but I forgot about Friction !! . Friction will generate compression in the tooths if the profile is not good enough and the contact is not point to point which is more prone to happen in my configuration.
4-I checked the brake to explore how stable was the tangential force (friction) . I finally chose three elements as it acts as a cushion.
During the process I realized that middle nodes do not adjust to the geometry no matter how many “Project on to surface” operation were done. Middle nodes are always in line with the main nodes.The longest the more mesh independent. Ideally a full ring would solve the problem but it introduced additional problems.
Regarding the other points that are more specific to the code and validation:
5- I’m considering single-tooth contact too but I should take a look at the last ISO 6336-3:2019.
6- Radius. Good point. I must check.
7-Stress. Maybe the most relevant point is about Stress result.
ISO Code provides Maximum Allowable Bending Stress and for me the equivalence with Principal Stress was not so obvious.
I noticed that the opposite root yield before the main one. That would deform the tooth which eventually would interfere in the next engage.
I guess the main concern for ISO is probably fatigue and crack initiation where bending/tensile stress governs.
Values would be: ( pending review of previous points)
Maximum Tooth Root Principal Stress=347 MPa
Max Expected Tooth-Root Stress sFP ISO 633-3 version ??? = 365MPa
I feel I’m inside experts’ area. I hope I don't end up screwed.
Thanks again Sebastianmaklary.
Regards
We do gears, and I would consider us "non-ISO hacks". But some things I have learned:
I take the time to make a good hex mesh. With some simple extrudes or slightly less simple sweeps for helical gears, you can get the basic shapes, then import a hi-res stl surface and use the project command to put nodes on the actual surface. Then you can study things like changes in crowning and similar.
If you output the stresses for each gear in its own cylindrical coordinate system, you can use the method I outline in https://mecway.com/forum/discussion/comment/4303 to calculate fatigue stresses. This is particularly useful if you have reversed loading on the gears.
Sorry if I'm dragging it too far away from the main subject of constraining movement but I just got excited when I saw a post on the subject of modeling gears.
1. Maximum bending stress and maximum contact (hertzian) pressure likely won't occur at the same contact location but frankly, I'm not too concerned with contact pressure. The reason for that being that I'm designing race car gearboxes so the consequence of pitting is considered less critical than root fracture since you can still finish a race with a damaged flank but a broken tooth will often result in a DNF. Also impacting my attitude towards contact fatigue is that we do not know the contact fatigue strength for the material in the condition we want to use. We know the strength for the base material with a polished surface but not in the hardened condition that we want to use. When I don't know the safe limits, it makes little sense to use extra development time to try to estimate what the actual contact stresses are.
Also, I suspect that the mesh needs to even finer than the one I have, if I want to use the output of that instead of the ISO 6336 method but since it is not my main interest, I haven't done mesh sensitivity studies with regards to the calculated contact pressure. To be able to calculate a line load, I have settled with a mesh that is fine enough that the contact spans 3-5 elements.
2. ISO 6336 also assumes 2-dimensionality and a plane stress condition so the importance of modelling as a 3-dimensional feature is more when one is concerned with using material strength data derived from non-gear tests or when one is concerned with the interaction of stresses between the gear root and the supporting material below it, if the gear isn't just a big solid. Also, if misalignments or tooth twists due to torsion input from one end is of interest as it is in the case of a gear that is wide in relation to its diameter, then the model must also be 3-dimensional as one end of the tooth will be loaded harder.
3. For root stresses, I think that Saint-Venant's principle applies and that having great accuracy in the contact isn't too important if the model is otherwise 2-dimensional. The friction will be very dependent on the surface quality, lubrication and temperature of the final object so being very precise with it in this stage of FEM isn't too important I think. I used a coefficient of friction of 0,1 but I am not sure if that is particularly realistic in a well lubricated gearbox.
4. Your brake confused me at first since I couldn't see a normal force that is supposed to cause the friction. Is it correctly understood that this normal force is supposed to be generated by the brake being modeled with a penetration through the ring?
5. The latest ISO 6336-3 includes some load-sharing in the calculation of the form factor Y_F but only when the contact ratio is more than 2. The contact ratio factor that I've seen in some books but not in ISO 6336 is Y_eps=0,25+0,75/epsilon_n, so with that factor, all gears with non-interrupted meshing would have their calculated stress reduced.
6. Geometry is important. Some checks you can do is to first see if it is a circular fillet and if it is, then check if the radius of it is the radius of the generating rack (as defined in standards), since that is a usual modeling error. The actual fillet of a regular generated tooth will have a radius that is larger than the tool that is making it because the tool rotates to make gears on a cylinder and then also, the fillet won't be circular.
7. ISO 6336 is normalizing the stress with the form factor and stress correction factor such that Ft/(b*m)*Y_F*Y_S and is doing so in such a way that the result of that calculation is the first pricipal stress in the tension fillet. In the introduction of ISO 6336-3:2006, it is described that while cracks may appear in the compression fillet, they won't usually grow and thus the tension fillet is much more likely to have cracks grow. From fracture mechanics, we also know that a crack in compression won't grow because it is being pushed shut while a crack in tension will grow because it is being pulled open, so this aligns with the statement in the introduction of ISO 6336-3:2006. Yielding is also often less important than fracture growth since the yielding (of an unhardened tooth) will likely be very localized to the surface of the fillet due to the stress concentration and thus isn't enough to deform the tooth enough to impact the function as it will just create some residual stresses upon unloading. I have however seen overloaded teeth that has yielded enough to destroy a whole gearbox without any teeth breaking but that has been a single overloading event from a messed up gearshift.
@JohnM I've also ended up being a "non-ISO hack" as all calculations based entirely on the ISO standard was unable to explain why the products we had bought was able to widthstand the loads they were observed to be able to. I found that it is both due to availability of materials that surpass that found in ISO 6336-5 and also because a much larger root fillets can be obtained by making custom tools based off of ones FEM analysis.
I think I should be able to make much better meshes as well if I put in more manual work into Mecway but that will have to wait until I find a better reason to do it. Perhaps if I need to do a more thorough analysis of the line loads, I'll do that to get better quality.
In this development project, I just had to quickly identify the best of about 6 geometries for just as many gear pairs so using time on something that could be discarded by an automatic mesh was not the best way forward.
Your mesh does look very nice and regular and I like that a lot.
I guess the gear study needs then to be performed in different positions depending on what it is evaluated.
4. Right. I can control Friction with the initial penetration and Normal stiffness per unit area. With just three elements it has shown to provide a very uniform and constant friction force. See image.
6. Still looking at this point. I do not recognize a clear radio on the .dfx file.
7. The point here is that as I’m not designing , I have set all factors to 1 so I’m not sure where should I look to compare, Principal stress or “uncorrected stress” like (VM).
I think that anyone considering if it is possible to design gears with Calculix/Mecway will have now a better understanding of capabilities and possible limitations.
It’s a pleasure to have people like you in the forum.
Thank you.
7. These factors are not 1 since they are what is describing the relationship between the stresses and the force, width and module so in some sense they are describing the (assumptions of) geometry and the load direction. It is how the stresses are non-dimensionalized so they are calculated based on the force, module, tooth width and all of the correction factors. My initial point about them was that they nondimensionalize the first principal stress and not the von mises stress, so for an FEM analysis to be compared to the ISO calculation, the first principal stress must be the output of the FEA.