Detailed gear parts affecting Onshape speed?

michael3424

I've imported some gear shapes into Onshape Part Studios and now my assembly is sluggish when I attempt to starting mating components together.

I used a program called Gearotic to specify the gear features (DP, # of teeth, and PA), exported that to a 2D DXF, imported the DXF into GeoMagic, to extrude the basic gear shape, exported the extrusion to STEP format and then uploaded that to OnShape, translated it and then did some minor revisions on the gears.  It looks like the gear generator produce a DXF file with tons of facets, so I'm assuming that is the source of the slowdown.  Does that make sense?

I've publicly shared a file with several of the gears in case anyone wants to take a look.

https://cad.onshape.com/documents/d3982d7a402e4578914f86f7/w/8778fb8636b344ee94b4b4ad/e/cec50dfdff994b62817e0be9

Mike

pete_yodis

Michael3424 said:

I've imported some gear shapes into Onshape Part Studios and now my assembly is sluggish when I attempt to starting mating components together.

I used a program called Gearotic to specify the gear features (DP, # of teeth, and PA), exported that to a 2D DXF, imported the DXF into GeoMagic, to extrude the basic gear shape, exported the extrusion to STEP format and then uploaded that to OnShape, translated it and then did some minor revisions on the gears.  It looks like the gear generator produce a DXF file with tons of facets, so I'm assuming that is the source of the slowdown.  Does that make sense?

I've publicly shared a file with several of the gears in case anyone wants to take a look.

https://cad.onshape.com/documents/d3982d7a402e4578914f86f7/w/8778fb8636b344ee94b4b4ad/e/cec50dfdff994b62817e0be9

Mike

@Michael3424 I suspect the problem lies in the approximation of the involute curve on the gear tooth flanks.  I used to generate 2D geometry in AutoCAD back in the day and then import it into SolidWorks and extrude to get a gear in 3D.  I would get a similar slow down in SolidWorks on large gears (lots of teeth) with a large amount of surfaces.  You are probably seeing a slow down because of the graphics burden happening when location and display of all those surfaces have to be handled.  I would try to have the gear tooth flank be all one spline that approximates the involute curve, rather than a series of segments.  This should do it.

ShepRCS

I generated my gears from scratch in OnShape.

Actually quite quick once you know the steps and results in 3 faces per tooth (5 including the fillets). which is quite manageable for me in terms of speed to mate etc.

I used this tutorial with the exception of the equations.  Worked well you can see my resultant model here.

Not a direct solution to your problem maybe but an alternative way of doing things.

Shep

michael3424

Thanks Shep - a procedure for designing for scratch was to be one of my follow ups so I've bookmarked that site and will look over your model later.  In the meantime I've downloaded CAD models of gears from Boston and Rush to move the project along and those seem to be a lot cleaner than the ones based on Gearotic .  Some of these gears are 14-1/2 PA, though, and downloads of them don't seem too common so I'll be trying out the method you referenced.

Nice model of the Elmer's engine by the way - have you built it?.  I have his book and my present Onshape project is a model of an 1867 Otto-Langen IC engine, which I'd like to build.

Mike

pete_yodis

Michael3424 said:

I've imported some gear shapes into Onshape Part Studios and now my assembly is sluggish when I attempt to starting mating components together.

I used a program called Gearotic to specify the gear features (DP, # of teeth, and PA), exported that to a 2D DXF, imported the DXF into GeoMagic, to extrude the basic gear shape, exported the extrusion to STEP format and then uploaded that to OnShape, translated it and then did some minor revisions on the gears.  It looks like the gear generator produce a DXF file with tons of facets, so I'm assuming that is the source of the slowdown.  Does that make sense?

I've publicly shared a file with several of the gears in case anyone wants to take a look.

https://cad.onshape.com/documents/d3982d7a402e4578914f86f7/w/8778fb8636b344ee94b4b4ad/e/cec50dfdff994b62817e0be9

Mike

@Michael3424 I suspect the problem lies in the approximation of the involute curve on the gear tooth flanks.  I used to generate 2D geometry in AutoCAD back in the day and then import it into SolidWorks and extrude to get a gear in 3D.  I would get a similar slow down in SolidWorks on large gears (lots of teeth) with a large amount of surfaces.  You are probably seeing a slow down because of the graphics burden happening when location and display of all those surfaces have to be handled.  I would try to have the gear tooth flank be all one spline that approximates the involute curve, rather than a series of segments.  This should do it.

ShepRCS

No not built it yet... Bit of a long story but I left Design Engineering  about two years after Uni, after I got a job offer that I couldn't refuse.  10 years later I'm trying to scratch the designing stuff itch.  Working on acquiring Lathe and Mill (or rather on the approval from other half) but in the meantime been modelling up some of Elmer's creations and at the same time converting them to Metric!  Good for getting my CAD brain back in gear and learning OnShape! Finished his Radial the other day but intend to get them all modelled and drawn up (once drawings are available) .

michael3424

Pete_Yodis said:

You are probably seeing a slow down because of the graphics burden happening when location and display of all those surfaces have to be handled.  I would try to have the gear tooth flank be all one spline that approximates the involute curve, rather than a series of segments.  This should do it.

Thanks - that's what I figured.  The Onshape system actually hung several times when working with a long gear rack and told me to restart but it kept hanging.  Creating tooth geometry from scratch for the rack in Onshape solved that issue but the spur gears made it far too slow to work with in the assembly.  Shep's reference should resolve that problem and in the meantime I am trying out gear models downloaded from manufactured, which seem much cleaner.

michael3424

@shep - another nice engine.  Designing the whole set is an ambitious goal.  There must be 50+ models in the book I have.

pete_yodis

@Michael3424 @Shep It would be nice in due time to be able to natively have Onshape produce true involute curves for gear design.  Probably a good idea for a company to do using the eventual Onshape API.  I looked at GearWorks years ago, but wasn't impressed that the geometry wasn't really true involute curves.  I'm sure the math and output into 2D/3D would not be easy.  You also have to ask the question is a true involute really needed, or is an efficient approximation all that's necessary?  Anyway, interesting topics...

michael3424

A gear-making module *would* be nice, but there's lots of other stuff that should have higher priority.  For the most part, approximations are fine for what I do, since the gears themselves would be made with form tools.  

pete_yodis

Michael3424 said:

A gear-making module *would* be nice, but there's lots of other stuff that should have higher priority.  For the most part, approximations are fine for what I do, since the gears themselves would be made with form tools.  

@Michael3424 I wasn't thinking of Onshape doing it, but a specialty company using the Onshape API to generate gears based on design layouts and calculations.

michael3424

@Pete_Yodis - that would be fine by me, too.  Even better since no Onshape resources would be needed.  It looks like Shep's approach will suffice in the mean time and that may be all that is needed.  

andrew_troup

Once Onshape can import dxf and other 2D input -- particularly if we can then do a 'fit spline' to replace polylines with clean single splines of suitably low degree -- then (at least for my purposes) a whole bunch of external toothspace generation options become viable.

michael3424

Do other CAD systems have a "fit spline to replace polylines" feature.  That could be handy in certain projects.

andrew_troup

@Michael3424 : Solidworks certainly has an effective "Fit Spline" command. Optionally it can retain the underlying geometry as construction entities, or replace them altogether. 

michael3424

@Andrew_Troup  - OK, so that's another area where Geomagic Design is deficient.

aaron_2

Go to www.rushgears.com you can download just about any gear you need in just about any format, and then customize in onshape. There is a limit to how many you can download in a day. They also have a gear builder.

michael3424

@aaron53560 - thanks!  I got a couple of gears that I needed from Rush but did not realize that they had a gear builder.  Onshape works much faster with the Rush & Boston gears than it did with the gears from converted 2D DXF files that I was using before.

aaron_2

Michael3424 said:

@aaron53560 - thanks!  I got a couple of gears that I needed from Rush but did not realize that they had a gear builder.  Onshape works much faster with the Rush & Boston gears than it did with the gears from converted 2D DXF files that I was using before.

Glad I could help, I know it worked great for me and took forever to find them. I only wish they had compound gears too.

dennis_20

In most cases a true involute gear profile is not necessary, just as in most cases a detailed helical thread is not necessary in a model.  However, there are those times when you not only need these features, but they must be dead-on.  SolidWorks has an involute function and I saw a demo of how to use it to make a gear profile, but there were several things I did not like about it.  The tutorial referenced by Shep on May 7 is a very good graphical method, but I developed something I like better.  Unfortunately for OnShape this technique utilizes a design table and more importantly, the calculations in its spreadsheet.  Now I just open my generic gear file, change its few parameters accordingly to get the basic gear I want and save it as the new name.  The technique uses an overkill of 19 points along the involute with a spline fit to it.  Now I have an accurate parametric model that is very easy to use.

I needed accurate gears that were a bit unusual: 14.5 degree, 0.6 module, stub tooth, for a prototype power tool and could not get them other than 3D printing (3D printed with a dental/jeweler's wax then investment cast in 17-7 stainless).  The solid models were perfect.  Without that the 3D printed parts would not have been possible.  Because of it I have a functioning prototype, not one that is just representative of the shape and appearance.

This is just one example of why I am particularly anxious for OnShape to provide the equivalence of SolidWorks' a) configurations, b) Design Table, c) equations, d) link to a spreadsheet.  Once this can be done in OnShape I would share the parametric file.