HELP! Gears (Globoids & Other types)

chandra_harsha

Hello folks,

I need help with creating various types of gears in Onshape. I am a Design Bureau, so work-around with circular arcs, or other methods will not work all the time, as I have clients sometimes ask involute profile on the gear. Please keep in mind about this, when giving me feedback/suggestions, and I appreciate your help.

Spur/Helical Gears  
I use Onshape Custom Tools "SPUR GEAR ( https://cad.onshape.com/documents/6527d86ca7126bbe5b04ca08/v/83e5f3eba1ab6d76e8deeb45/e/3ea2b29bac4713685544dc37 )" & "PLANETARY GEARS ( https://cad.onshape.com/documents/b55a80bb510b8ff5cb20fd9a/v/48a8d665dd43d50680e9ca65/e/24256daec5d2bac4406f58d6 )" to generate these type of gears. I assumed they already follow involute profile, and helix profiles. I have two limitations with these tools:

Ring Gear: I have to manually generate Ring gear most of the time. As extracting Ring Gear from "PLANETARY GEARS" tools is tricky sometimes. I generally calculate module of gear set, and create a normal spur gear with tooth number near to my calculations, and then project sketch of single tooth on Ring gear pitch circle, and create gear from that. Is there any specific custom tool for creating Ring Gears?   

Teeth more than 1000: Sometimes I have design inputs like, "shaft/ring thickness of 4mm, with 3mm gear tooth height", and I have instances where sometimes calculations show tooth number like 1300. I know this is rare, but this happens with some R&D projects, where ideas are being explored. In tools mentioned above, current limit on teeth number is 1000. So, again I create sketches with pitch circle and other gear parameters, and copy sketch of one tooth from smaller with same module, and paste it on required gear pitch circle. However Onshape has difficulties in multiplying features in these numbers (checked with support and confirmed this, and they also provided some suggestions on how to approach this), and so document goes into forever reload, when I do circular pattern on tooth. Instead, I create gear blank and tooth as separate parts, and create a assembly with these in exact same position, and do circular pattern in assembly. I do same colour to both, so it looks like gear. This is faster, and doesn't break files. I want to ask others is there any other methods people are using for these kind of situations?  


Of other type of gears (except Worm Gears & Globoids), I didn't work on designing them yet, but I would like to ask, if there are any specific customs tools out there, for Bevel gears, Hypoid, etc. 


Worm & Worm-Gear
Like explained above, I do calculations, and create a spur gear for worm-gear, and copy one of its teeth to create worm using loft. This kind of worked, as these models are not used to create production drawings, or something like that. Things like throat, or if helical gear is involved as worm-gear, I haven't tried creating those. Tricky thing is, addendum to dedendum ratio in worm-gear setup is different to spur gears, and also have variations to it, depending on lead angle. So, my method of creating worm-gear set up is not accurate. Any suggestions here?


Globoid  
On one of my current projects, I was asked to size and design globoid-gear in initial design. I felt embarrassed  to not know what it is, and how to create that. I still didn't succeed in creating this, but tried few things as explained below:

• Like in worm-gear, I created globoid blank with root circle (calculated), and created a helix at pitch diameter. Now what I wanted to do is, project this helix onto globoid blank (image below), and loft like normal worm gear. This is not a perfect globoid, but would work for now. But I couldn't proceed further because I am unable to project helix onto globoid blank. I didn't explore much here, as I found other methods like explained below, which I didn't succeed as well

• I also thought, creating a variable radii helix using "Parametric Equation curve ( https://cad.onshape.com/documents/578ff8b3e4b0e65410fcfda3/w/d33395f174e5b38f4abd6097/e/cc0c3d5644a78b1b64d6c3b4 )", and using equations mentioned in link https://www.zwsoft.com/support/zw3d-base-skills/1378 . This will be my last ditch option. I have to dust off my math, but I am wondering surface on which this helix sits is a cone, but globoid surface (root dia) is not cone, and has curvature. Thats why I didn't explore this option completely 

• I checked Onshape forums, and came across a discussion, where @konstantin_shiriazdanov posted few suggestions. https://forum.onshape.com/discussion/13641/globoid-thread He shared a file that contains his work on globoid creation but I couldn't make "Curve Generator  https://cad.onshape.com/documents/d8aab1e0e7ae10038a6830e0/v/5c9f65e4909a623a7644a665/e/421758eb171fa79c9a45f9a6 " tool work. I couldn't get my head around it, and figure out how it works 

• I also came across this link https://spiralbevel.com/ , and thought of following their method, but their excel sheet that generates tooth curve is not available

So, with this, I need some help on how to create a globoid. I am still trying but didn't succeed yet. I read some papers on globoid tooth profile mathematical equations, but didn't get much time to understand them properly.


Another thing, generally I consult "Shigley's Mechanical Engineering Design" to verify my calculations. It has some good explanations, majorly for spur/helical gears, with some inputs in bevel and worm gears too. But if someone can suggest me a book that has some thorough reasoning on all kinds of gears & design, with their parameters, equations, etc. I would appreciate that.

Thanks,
Chandra
    

konstantin_shiriazdanov

If gear design is your company buisness I would really recommend you to find a production-ready solution. Spiral-bevel looks good for me and should be pretty affordable, you may contact him and ask if the globoid gearing generator is available.

S1mon

Realistically, you may want to ask yourself what your goals are in modeling a gear in a generalized CAD tool.

1. Is this just visual for reference and you're buying off-the-shelf parts?
2. Is this something which will just be 3D printed for fun?
3. Is this for a one-off machine, or a high volume consumer or medical product?
4. Will these gears be machined or injection molded?
5. Will the gears be metal or plastic?
6. How small are the teeth?
7. Are you trying to do FEA on the models?

In my experience, hiring a professional gear designer who uses specialized CAD tools is essential for good performance, especially with molded gears (gating, shrink and draft on plastic gear teeth has complex effects on noise, wear, and torque). Similarly, tool design and molding for plastic gears is not something you want to hand off to any random injection molder.

If it's a metal gear, chances are good that the manufacturer will use specialized gear cutting tools which will help to create the profiles you need.

Drawings and inspection of gears also requires specialized tools and techniques. If you don't know what to ask for you may get something that kinda works like a gear, but doesn't perform very well.

nick_papageorge073

The above two comments have paralleled my experiences. I designed a few transmissions for children's products years ago. The gear world is very specialized, and all the gear vendors have their own tooth shape generating software, their own specialized measuring systems against a master gear, etc. The solutions I've seen for general CAD systems like OS were very basic. They don't have things like profile shifting, for example, which you need to prevent undercutting and maintain tooth strength if the number of teeth gets too low. Anytime I did a gear, I would draw it as a simple cylinder at the pitch circle diameter.

chandra_harsha

@konstantin_shiriazdanov , ok. We are just looking at different ways in designing gears in Onshape. We leave production ready gear designs to expert people in that. In your Globoid gear public document, you used a custom tool called "Curve Generator" , if possible can you please let me know how it works? Thats where I got stuck in your document. Thanks.

@S1mon & @nick_papageorge073 Thanks for your inputs. Like you said, when it comes to exact gear design, I leave it to respective manufacturer for actual design. In the past, when there is a gear, I generally make cylinders with pitch circle, to mimic gears (with other features that are important for its fixation, etc). But recently, some of the clients started asking gear in the design to be more representative of actual piece. Spur Gear tool works for most of my cases, but I had instances like once, a client asked me he wants a hypoid gear, and teeth to be with involute profile. 

About those Globoid gears, I can't go into exact specifics, but we are in preliminary stage in R&D on a certain project, and we need teeth and approximate representation, because we are trying to estimate weight (very critical to application) of assembly. So, similar method to worm-gear (my method) should help, even though teeth is not same as spur teeth, but I couldn't get the helix (spiral) required for loft in globoid case. So, yeah I am looking for approximate designs in this case.

I created this thread, to gain some knowledge on how different designers are approaching gear designs. Also designing gears felt a bit challenging , and made me curious. 

konstantin_shiriazdanov

Curve generator creates a trajectory of a point which position depends on some numeric variable by creating a number of those point instances corresponding to the different values of the driving variable and creating a spline through those point coordinates. In the case of globoid worm trajectory we have some point of the wheel pitch circle whose trajectory need to be captured. This motion can be decomposed as simultaneous rotation around wheel axis and rotation around worm axis while rotation angles are constrained by the constant gear ratio. To define trajectory relatively to some moving coordinate system rigidly connected with the worm body with Curve generator feature I did the following:

created a variable which represents rotation angle of the wheel #phi, created a mate connector on the worm axis and set its rotation around Z axis at #phi*#u angle (#u is gear ratio) defined a sketch with a point on wheel pitch circle and constrained point position to be at #phi polar angle from the perpendicular to worm axis (here you should make sure that all sketch constraints to the external entities are fixed with sketch fix constrain otherwise sketch will rebuild unpredictably ). And here you are -  call the Curve generator, select the sketch with the point whose trajectory you want, check "use local coordinate system" and select the mate connector which represents worm coordinate system, fill the name of driving variable "phi", set the range min/max values and step and it should work.

EvanReese

@rodrigo_rivas_costa made this globoid gear feature. As with anything open source, I'd double check the output, but it looks pretty good to me.

chandra_harsha

@Evan_Reese Thank you . That kind of tool works for most of my designs. I have few questions, but I will check with the person that created it about that.

@konstantin_shiriazdanov I didn't get time to work on your method, but I noticed I didn't use fix constraints in sketches. I will explore this further, and if I have more questions, I will post in this thread. Thanks again.

rodrigo_rivas_costa

chandra_harsha said:

That kind of tool works for most of my designs. I have few questions, but I will check with the person that created it about that.

Hi! I'm the creator of that feature. I'm happy it helps you. If you have any question just post it here or feel free to send me a private message.

chandra_harsha

@rodrigo_rivas_costa Thanks for your help! 

Can you please tell me what does parameters "Screw Padding" , "Fall off" , "Vertices per Screw Loop" do? Or how we can use them to tailor your needs?

rodrigo_rivas_costa

chandra_harsha said:

Can you please tell me what does parameters "Screw Padding" , "Fall off" , "Vertices per Screw Loop" do? Or how we can use them to tailor your needs?

Sure!

"Fall off" affects how the spiral thread of the screw ends, since it has to end somewhere. If it is 0, then the thread ends abruptly, as a square cut. This can be an issue, particularly if you have some backslash, because the sharp edges can "bite" the teeth of the gear. A value of 0 means that the fall-off is disable. A positive value is the exponent of a "sigma" like function that smooths that cut. WARNING: Actually a higher value means a stepper cut, so a 1 will be super-smooth, while a 5 or a 10 will be nicer. Also note that the end of the thread is somewhat retracted by the fall-off.

"Screw padding" is the distance between the end of the screw thread and the top/bottom of the screw body. Yes, you could just extrude the cap, but that would not follow the nice curve of the screw body.

 

It is also useful if you want to chamfer or fillet the edge, as it can get quite sharp. Without the padding the chamfer would overlap the thread and fail.

"Vertices per Screw Loop" is used to build the thread spiral. This thread is built as a loft of a lot of small tooth profiles around the body of the screw. How many profiles? Well, as many as this parameter says, per loop. If you set "Vertices Per Screw Loop"=16 and "Teeth in Screw"=7, then the screw thread will be built using 16*7 = 112 profiles. A higher value means a more precise shape, but at the cost of more computation, memory and render time. Here is a view of the generator profiles with the screw hidden:

I hope this helps.

rodrigo_rivas_costa

Now I remember, I added "screw padding" because the screw border can get quite sharp, but if you try to chamfer this border without a padding, it will not work, because it will conflict with the end of the thread.

chandra_harsha

@rodrigo_rivas_costa Thanks for your comments. "Screw Padding" is very useful, to manually create that extension to screw surface needs few operations and gear calculations. Same with "Fall off", I tried to smooth the end of globoid teeth manually, but its very strenuous, making lot of unnecessary (in terms of complete design) arcs. 

About limit, not just on your tool (I checked your FS), but also actual "Gear" & "Planetary Gear" tools in Onshape, why teeth is limited to only 1000. I know you rarely go beyond that, but I am working on a project where we are assessing a design of an assembly with some titanium gears with CF base, in which I have more than 1000 teeth. Is there any particular reason why 1000 is the limit for gear tooth generation in Onshape?   

konstantin_shiriazdanov

chandra_harsha said:

Is there any particular reason why 1000 is the limit for gear tooth generation in Onshape?   

It is likely for performance reasons, you can try to copy that feature and edit bound spec of corresponding input for the higher upper bound value

rodrigo_rivas_costa

chandra_harsha said:

About limit, not just on your tool (I checked your FS), but also actual "Gear" & "Planetary Gear" tools in Onshape, why teeth is limited to only 1000.  

My reason to choose 1000 is that I copied the "bounds spec" from the other feature scripts, without thinking too much about it. Not setting a limit is dangerous, because if you accidentally hit Ctrl+V twice and paste 100100 you may have an OutOfMemory situation and hang your browser.

That said, you can private copy my FS and custimize it, or if you prefer, I can bump up the limit to any other reasonable number.

rodrigo_rivas_costa

There is an issue here, that happens with more than 85 teeth. The thing is that I'm building just one tooth, and then multiplying it using a circular pattern. With too many teeth the circular pattern fails because of a geometrical instability in the axis edge, too narrow, I think.

So, @chandra_harsha, please check V4 with a bigger tooth limit (10000) and a hole in the middle. I've added a new parameter "Axis hole (percent)" to set up the hole. By default is 5%, but you can set it to 0% to your own peril, because not having it may cause the gear to fail randomly. Or you can always fill the hole with an extrude later.

And just for show, here is a worm gear with 1000 teeth

chandra_harsha

rodrigo_rivas_costa said:

There is an issue here, that happens with more than 85 teeth. The thing is that I'm building just one tooth, and then multiplying it using a circular pattern. With too many teeth the circular pattern fails because of a geometrical instability in the axis edge, too narrow, I think.

So, @chandra_harsha, please check V4 with a bigger tooth limit (10000) and a hole in the middle. I've added a new parameter "Axis hole (percent)" to set up the hole. By default is 5%, but you can set it to 0% to your own peril, because not having it may cause the gear to fail randomly. Or you can always fill the hole with an extrude later.

And just for show, here is a worm gear with 1000 teeth

That explains why I had trouble getting larger gears created using this tool. Nice that you found where the problem coming from. 
I am new to FS, so didn't know about this "bounds spec". I will update to your current version.
To give you an idea, my parameters wrt tool inputs are as follows:
px = 0.10923in, so module m = 0.03477in
teeth in gear = 1275
gear width = 1-1.5in (currently I kept my models with 1in width)
attack angle = 20deg
teeth in screw = 10in/px =  91.54, so 91 teeth, as I need globoid screw to be around 10in long
screw diameter = 2.7405in (pitch diameter of screw) 
I will try to recreate my models and get back to you.