Saturday, January 13, 2018

Making gears for 3D printing using Autodesk Inventor

You want to design your own thing that you're going to 3D print, and it's going to have gears.  Awesome!  It's probably going to be something great.  Being able to design gears for 3D printing is a super useful skill, but if you don't know anything about gears it could be a little more complicated than you might expect.  I'm going to tell you what I know about gears, and how to design them for use in your 3D printed project using Autodesk Inventor.

I can hear what you're thinking right now:  "What?!? Inventor?!?  Do you think I'm made of money?!?  Why don't you show me how to make gears in Fusion 360?"  Let me tell you I would LOVE to show you how to make involute gears in Fusion, but I don't know how.  I've done some cursory research, and no other software makes generating custom involute gears as easy as Inventor, free or expensive.  Also, Inventor is free for students and teachers, so hopefully you fall into one of those categories, or at least can convince Autodesk that you do.

First, lets get the vocabulary out of the way.  There is a ton of gear vocabulary, but I'm only going to discuss the minimum that we need to know to make the gears.

Pitch Diameter: This is the diameter of your gears if the gear teeth were infinitely small.  In other words, if your gears were perfect cylinders with perfect friction on each other, the diameter of these cylinders would be the pitch diameter.  When designing gears from scratch, without the help of a $1,890 (per year!) piece of software, the pitch diameter is our most important dimension.  In Inventor though, it won't be that important to know.

Center Distance: Half of the pitch diameter of the first gear plus half of the pitch diameter of the second gear would give you the distance from the center of one gear to the other.  If you have two shafts, and you want to connect them with gears, the center distance is how far apart those shafts will be.

Outside Diameter: This is the diameter of the circle that makes up the tops of the teeth.  It isn't important in any of our calculations, but it is important if our gears are going to fit into a housing.

Pinion: This is the name of the smaller of two mating gears.  The other one is just called the gear.

Diametral Pitch: This describes the size of the teeth.  The units are generally teeth per inch of pitch diameter.  The bigger this number is the smaller the teeth are.  Must be a whole number.  Common pitch sizes in radio controlled cars are 32, 48, and 64.  Both mating gears must have the same pitch.

Module: This does the same thing as diametral pitch, which is to describe the size of the teeth, but with metric units and as a ratio.  It is the number of millimeters of pitch diameter divided by the number of teeth.  LEGO Technic gears have a module of 1.  So, the LEGO 24 tooth gear has a pitch diameter of 24mm.  I almost always design my gears with module instead of diaetral pitch, even though I design everything else in inches.  I have learned that the smallest consistently trouble-free teeth that I can 3D print are a module of 1. 

Backlash: This is how much a gear can rotate when the other gear is being held still.  If there is no backlash there will be excessive friction.  Backlash is important in 3D printed gears, because it is difficult to control if the parts are slightly oversized or undersized.  My 3D printer almost always makes my gear teeth just a hair too big, and I compensate by adjusting my backlash.

Involute: An involute shape is a part of a spiral.  Why is this important?  Because the sides of the teeth are actually not flat, like you might imagine, but rather curved in an involute shape.  This is a difficult shape to manually draw in a computer aided drafting program, but Inventor will take care of this for us.

It's not obvious, but if the sides of the teeth were flat, they would CLACK against each other when their faces met, and the tips of the faces would drag across the mating faces, causing excessive friction.  The beautiful thing about the involute shape as a tooth surface is that it causes the mating teeth faces to "roll" on each other instead of sliding.  This is absolutely critical in an actual working gear for mostly silent, nearly friction free operation.

Pressure Angle:  This describes the angle that the teeth surfaces press against each other at.  There are two common options, 14.5 and 20.  I have always used 20°, but I am planning on experimenting with 14.5°.  Mating gears should have the same pressure angle.

Helix Angle:  Some gear teeth are not parallel to the axis of rotation, but rather wrap around the gear diameter at an angle, sort of like a slight spiral.
The benefit of this is that it causes much less noise and friction.  Almost all automotive gears are helical these days, except for the reverse gear in manual transmissions, which is straight cut, and is why your gears sound like they are "whining" in reverse.  The drawback is that the gears want to "unscrew" from each other, which makes them push in opposite directions along their axis of rotation.  This makes it so that you need thrust bearings to keep them in place.  In 3D printed applications this is generally impractical. It is possible to put two opposite-angled helical gears together to form a single gear, which is called a herringbone gear. 

It has all of the benefits of a helical gear but none of the drawbacks.  They are very difficult and expensive to machine, but just as easy to 3D print as any other kind.  They have the additional benefit of keeping the gears aligned with each other, which can often be used to simplify other parts of the gear train design.

On to Inventor!

You might assume that you would design two gears as separate parts and then put them together in an assembly file, because that’s the way everything else is done in Inventor, but you would be wrong.  Gears designed in Inventor’s gear generator tool are designed in an assembly file, and the part files are generated automatically.  So, the first thing we need to do is make a new assembly file, and then save it.

Next, we will go to the Design tab, and click on the Spur Gear generator button.  You may see that there are also options for generating bevel gears and worm gears, but neither of these options are able to generate functioning 3D printable parts.  They are for representing parts that they assume you are going to purchase.  The spur gear generator is the same way, but at the end there is a trick for turning them in to useful parts.

Once the window pops up, make sure you click on all three window expanders: the one to the right of the main area, the one below the main area (but above the Calculate/OK/Cancel buttons), and the one to the right of the Cancel button.

Now we have to make some decisions. 
1) Do you want to use diametral pitch or module?  Like I said earlier, I make all of my gears using the module system of tooth sizing.  I am very happy with a module of 1mm for 3D printing.  Click the radio button under Size Type to make your choice.
2) Do you want to tell Inventor how many teeth each gear needs to have, or simply what the gear ratio is?  I like to specify the number of teeth because when I’m designing my gears, I don’t usually have the parts that hold the gear shafts designed yet, and I can put them wherever they want.  Because I know my tooth size module (usually 1mm for me) and the number of teeth, that is how I control my center distance later.  This plan may not work for you, but that’s what I do.  Make this choice with the Input Type radio buttons.
You need to make choices 1 and 2 before you go on to make choice 3.
3) Inventor is going to end up calculating SOMETHING for you.  What do you want it to be?  Your choices are under the Design Guide dropdown.  I nearly always make my choice as Center Distance.  This means I say what my module is, how many teeth each of my gears have, and Inventor uses these two inputs to calculate my center distance.  If I don’t like the center distance that it calculates for me, I change the number of teeth on my gears until it’s what I want.  I have found this to be by far the easiest method of designing gears, but it requires that I don’t have a center distance that is fixed. 
If you have a center distance that must absolutely be held, you can chose one of the other options and let Inventor calculate what your module, tooth count, or module AND tooth count is.  There is another option for Total Unit Correction, but I don’t know what that does, and I’ve never used it.  In fact, any time there’s a box for Unit Corrections anywhere in this process, I leave it alone. 
Once your big three choices have been made, you should go ahead and change your pressure angle to 20 or 14.5 degrees (I’ve always used 20), and change your Helix Angle to zero, even if you are going to actually make a 3D printable helix gear.  (We’ll do the helix part later with the coil command, if that’s what you’re into.)

Make sure you unclick the Internal checkbox, unless you want internal gears.  Inventor can make them, and they work, but I have found them to be finicky with regard to their smoothness and center distance.

You can set your Facewidth of both Gear1 and Gear2 to be however thick you want them.

Next, enter how many teeth you want on Gear1 and on Gear2.  Make Gear1 be the smaller number if the two gears do not have the same number of teeth.  In other words, make Gear1 be the pinion.   This will help you keep track of things later.

Ignore the Cylindrical Face and Start Plane buttons.  Inventor can design gears into an assembly in which you have already defined the gear axis and face planes, but I’ve never done that.  It seems complicated.

At this point you should be able to hit the Calculate button, and the Inventor calculated fields will update.  I have never in my life had Inventor think that my gears were going to work.  It always says, in red text, “Calculation indicates design failure!”  Yet, they always seem to work just fine.  There is probably a way to dig deep into Inventor and fix this, but it’s the easiest to just ignore it. 

After that you can hit the OK button, and Inventor will open up a window allowing you to rename the gear files (but I just keep the default names Inventor gives them), then another giving you that same warning again; just hit Accept.  At this point you will place the two gears, as an assembly, into your assembly file.  If you zoom in to the meshed teeth, you will see that these teeth are interfering with each other, and that they have a very simplified face profile.  THESE GEARS ARE FOR VISUAL REPRESENTATION ONLY!  Involute teeth are very complicated, and if Inventor went and put in a bunch of mathematically complex parts into moving assemblies, it would bog down computers badly when they were rotated.  Furthermore, it’s a pretty safe assumption that most people are buying their gears from a gear supplier, and it’s a waste of processing power to needlessly over-complicate them here. 

We do need them with a true involute profile though, so what you are going to do is to right-click on one of the two gears, and choose Export tooth shape.  A window will pop up asking you if you want to export the tooth shape of the pinion or the gear, and what kind and how much backlash you want.  I normally leave it at Normal, and I make the backlash as big as I can (before Inventor changes the field text to red, meaning it won't work), which is often about .006”.  I think my 3D printer over-extrudes, so I need my teeth to be thinner than they should be, and even with my biggest backlash sometimes my teeth mesh too tight and I have to adjust the center distance in my assembly that holds the gear axles. 

Once you have done that, click OK, and Inventor will open you a new part, which is a cylinder with a sketch, not of the tooth, but of the space between two teeth.

What you need to do is make that area a cutting extrusion, all the way through.

After you have done that, you need to make a circular pattern of that feature, and array it the number of teeth that are on that gear.

Technically you have a working 3D printable gear now, but really you need to draw a hole in the middle of it and extrude it through so that it can either slip fit onto an axle, or press fit onto an axle. 

Tips and tricks:

If you want to design a compound gear (a single part with two different gears stuck together side by side) for 3D printing, the best way to do it is to make two different involute toothed gear part files, then stick them together in an assembly, and make an .stl file out of the assembly.

If you want to make herringbone gears, make your facewidth half as big as you really want it to be, and instead of using the extrude command to cut your space between the tooth, use the coil command to cut it into a spiral.  Make sure you spiral both Gear1 and Gear2 the same angle.  Make the circular pattern of the spiral tooth space.  Then make a derived part of Gear1, making it a mirror of the original part.  Finally, make an assembly of the gear and the mirrored derived gear, and there's your herringbone gear.

It is extremely unlikely that you are going to be able to use the center distance that Inventor calculates for you as your true center distance in the real world with 3D printed gears.  I ALWAYS make my gear shafts adjustable so that I can fine tune the real-life center distance for optimum gear engagement. 

If you want to make bevel gears with a true involute tooth shape, check out my blog post on how to do that. 

Useful Links:

Saturday, November 11, 2017

Building a Canoe Paddle

Aside from building things, my main recreational activity is canoeing.  I paddle mostly on rivers that are shallow and rocky, so I split a lot of paddles.  I typically buy the Bending Branches Loon model.  It's cheapish and light, feels good in my hands, and I can buy them locally.  I really wanted to make my own paddle though, so that's what I did.  I teach high school wood shop, and one of the great benefits is that I have a really awesome wood shop all to myself in the summer.

The first thing I did was to watch the How it's Made video on canoe paddles.  It turns out this is Grey Owl's facility, and I think they are making the Voyageur in this video.  I mostly did it the way they do it, with some adjustments to suit my tool availability.

I also watched this video from Sanborn Canoe Co.  I mostly didn't do what they do, but I really like the way their paddles turn out, and I would like to incorporate more of their techniques in my future builds.

First, I glued up the blade halves.  This looks like it's going to end up as a single glued piece of wood, but there's no glue between the two middle pieces of walnut.  For my blade I used walnut closest to the shaft, then cherry, then some more walnut, then maple on the outsides for impact resistance.  My paddles get beat up on the sides of the blade the worst.
Gluing the blade halves
 While that was drying, I glued the shaft.  It is made of basswood for light weight and stability, with a walnut stringer down the middle.  The 1/16" walnut sliver was the hardest part of the entire woodworking project.  At the time I didn't have a drum sander, so I had to cut it perfectly on the table saw.  I really dislike cutting thin things on the table saw (and the only piece of walnut that I had at the time was warped enough that planing it flat would have made it nearly non-existent).  Now that I have a drum sander I would have cut this piece on the band saw and sanded it flat, but it worked out OK anyway.  I glued it all against the table to keep it straight.
Gluing the shaft
 After a few hours I glued it all together, including a few pieces for the handle.  I intentionally left the handle long on the blade end for two reasons.  The first is that my thickness planer snipes badly, and I wanted it to snipe that leftover part instead of the blade.  The second will become apparent when we get to the CNC shaping of the blade.
Gluing it all together
 I made sure the handle matched the wood on the blade.
Future handle
 After it dried for a few hours I ran it through the planer, taking off only what I needed to get it flat.
Thickness planer action
 At this point I got really excited.  If I had to do it again, I would have used single pieces of cherry on the blade instead of the two pieces glued together, or put a maple sliver between the pieces.  Not a giant deal, but next time.
Looking good
 Here's the handle.
 The next step was to cut the profile, but I didn't cut the end of the blade.  This is for when I shape the blade on the CNC, after I flip it over it will still lay flat.  Pictures below.  Note that the shaft is thinner than the shaft glue-up.  It is 1" wide, and I planed the whole thing to 1.25" thick, to match the handle of the Bending Branches Loon that I currently use and like.
Mostly cut out on the bandsaw

Cutting straight lines on the shaft was hard for me
 Next I routered the whole thing, both sides, with a half inch round-over bit  This was mostly to shape the shaft and handle, and to provide a neat transition between the shape of the shaft and the upcoming blade taper.  I wish I had a quarter-oval bit that would make the shaft oval instead of a rectangle with rounded corners, but I've never seen one.  I could use a custom shaper blade like in the How It's Made video, but it's probably not worth it at this point.  I would really love to hand shape the shaft with drawkinves and spokeshaves, but while I have both of these tools, I'm not yet adept enough at sharpening the blades to make them work well.
Beginnings of a nice shape to the walnut piece

Basswood burns badly when routering its endgrain, apparently
 Before I was a wood shop teacher I was a drafter, and I teach some computer aided drafting classes too.  I used these skills to model my paddle blade in Autodesk Inventor, then use the (awesome) Inventor HSM to make the g-code to shape the taper of the paddle.  I would like to make the taper a more complex shape and add a small spine with the shaft transition, but I decided to keep it shaped like the Loon that I know works well for me.  I have read that a spine can cause flutter if not shaped correctly, but mostly I'm lazy and I just wanted to get this done.
On the CNC!
 Here is a shot that shows the main reason I kept the blade too long.  If I hadn't, when I flipped it over to cut the other side it would have been difficult to hold to the table.  If I didn't have a CNC, I would have cut it on a bandsaw, on its side.  I doubt I would have been able to do as good of a job as the robot though.  Again, someday I hope to be able to hand shape all of this with planes, chisels, and spokeshaves.  They say, "To a man with a hammer, every problem looks like a nail."  My hammer is my CNC.
Still with the leftover on
 At this point it looked like a paddle, and I was very excited.  There was a LOT of sanding to do, and I was envious of the folks in the How It's Made video's giant belt sanders.
Looks like a paddle!
 I was very excited about the way the wood joints curved, and spent a lot of time making sure the transition between the shaft's 1/2" router shape and the blade taper looked good.
Walnut brings out a nice shape
 I have a 2" diameter oscillating spindle sander that I used to shape the finger and palm part of the handle.  I think it turned out particularly nice.  I was very happy that I spent the time to get that sliver of walnut down the center cut and glued in the handle.  It brings out the shape nicely.
The handle
 My next step was to give it some tip protection.  I beat the daylight out of the blade tips of my paddles, and if I had left this paddle as is, it would split and dent, especially where the soft basswood is exposed in the middle.  I decided to make an ash tip guard, and I wanted it to be connected with a tenon and lots of glue surface.  It took a long time to plan, but I decided on a two-part tip with a two-step glue-up.  Here is the first half of the tip after being cut on the CNC.
Half of the ash tip guard
 Then I cut the mating profile onto the blade.  The walnut strip down the middle made positioning the bit in the middle of the blade much easier when I started the program.
Cutting half the tenon
 Next I glued the two pieces together.  They are being clamped up and down, and also along the length of the shaft.  I built a clamping point out of 2x4s to pull against.
Will the gluing never end?
 Then I cut the other half of the tenon on the CNC.
2nd half of the tenon
 At this point I shaped the end of the blade to its final shape.  This would help guide me in knowing where to cut the second half off at, as the tip of the blade wood would be hidden after the next gluing.
Final blade shape
 this is the CNC of the other half of the tip guard.  Note that it does not have a step, so the two pieces of ash will not be glued along the centerline of the blade, but rather offset along one side of the tenon.
More tip guard wood

Here's how it will fit.
 More gluing.
Gluing never ends
 While I was waiting for the last of the glue to dry, I CNC cut this piece out of a 2x4.  It has an elliptical profile, and I used it with sandpaper to give my shaft a more pleasing profile.  It's like a poor man's shaper.
Shaft elliptification
 At this point I could hardly wait any more.
 After the glue had "dried"
Impatient woodworking
 Finally it was time for the big hand sander for final shaping.  Things went fairly quickly.
Belt sander ftw
 Next time I want to make the middle lump pointy-er.
It ended up looking pretty good


You can't really see the glue line between the two pieces of ash
 I needed to fiberglass the sides of the blade for strength, and I have a laser cutter, so why not cut the fiberglass on the laser?  Lots of reasons, it turns out, but I didn't know them at this time.  Don't do this.  The edges burn ever so slightly.  Not everywhere, but enough places that it took some time to cut out the burned parts with scissors, which sort of made the laser cutting pointless.  That wasn't the main reason though.  More below.  Also, the fiberglass you buy at Lowes is 6 oz. fiberglass, which holds way too much resin and adds weight.  4 oz. would have been better, or even less.
Laser cut fiberglass cloth.
 Speaking of lasers, I used the engraver to burn my name and a logo into the basswood, which turned out nice.  You have to trick this unit into thinking the front door is closed with magnets.
 I mostly canoe the Buffalo National River in Arkansas, and it's thanks to the hard work of Neil Compton (along with many others too) that we have this treasure.  They fought for years before I was ever born to save it from being dammed.  He is no longer with us, but his canoe is on display in Bentonville and it has this triangle pattern panted on it.  I decided to engrave it into my paddle as an homage to him.
Thanks Neil!
 Everything had gone really well, and worked on the first try, up until this point.  We are now two days into fabricating this paddle, but the rest of the job would take a week and a half.  I want to express at this point how much I dislike the process of fiberglassing.  It's important, however, for the lifespan of the paddle.  You can make the blade much thinner if you strengthen it with fiberglass, which saves weight and allows it to slice through the water easier.  I decided to use epoxy resin instead of the more "normal" polyester resin because it's supposed to stick to wood better.  I had used Bondo polyester resin (which I bought at Lowes) to repair a paddle once, and it worked, but indeed it delaminated from the wood in several places after time and abuse.  The epoxy had almost no odor, which was great, as polyester resin smells truly awful.  I used Evercoat because I was able to buy it locally, although it was a hassle finding it.  Nobody stocks epoxy resin, it seems.  Epoxy resin costs WAY more than polyester resin.  Since completion I have been recommended to use U.S. Composites 635 thin epoxy resin, and it is much cheaper than most I have found.
 Here is what NOT to do.  I put the cloth on the face of the paddle, then poured the resin over it, like I saw on a YouTube video.  I should have read the comments though because after I went back when this day was over and watched it again they all said not to do this.  The cloth will float on the resin, which makes a space under it full of resin which adds weight but not strength, and will make the face look lumpy and not smooth.
Don't do this

Ugh.  Lumpy.
 What you SHOULD do is paint down a thin coat of resin, roll the fiberglass cloth onto it to stick it down, then add a bit more resin to fill the cloth.  That's what I did on the other side and it worked great.  Here's the problem with the laser cut cloth though, and that's that it should have overlapped the edges so that I could have cleanly sanded them down when the epoxy hardened.  Instead I got this annoying ridge all the way around, near the edges, that took a ton of time and resin to fill.
Laser cut fiberglass equals misery
I was also distressed to find that the epoxy resin darkened the basswood significantly.  I lost a lot of the contrast in the wood that I liked, but I guess I should have expected it, as it ended up similar in tone to my current basswood paddles.  I'm not sure what I'm going to do about that in the future.
White wood is now tan wood
 It took a lot of sanding and adding more epoxy, then sanding more before things started looking good again.  Every coat took 24 hours before it could be sanded too.  Ugh.
Before the final epoxy coats
 I ended up having major fish-eye problems with my epoxy, and I never did figure out why.  Eventually I just stopped adding coats and brushed a final coat of Minwax water based Spar Urethane over everything for UV protection.  It turned out all right I guess, but it was way more work than it should have been.
 I didn't weigh it before the fiberglass, but it sure did feel heavier afterwards.  One pound thirteen ounces isn't terrible, but it's heavier than I wanted.  I could have thinned the blade more, I think, and that's where you want the weight reduced.
A tad on the heavy side
 Overall I'm happy with the way it turned out.  I'm going to try to use and abuse it like a normal paddle.  It's been a fairly dry late summer and fall paddling season though, so even though it's November now, I still haven't had a chance to try it out.

Since I built this one, I mostly completed another paddle, made mostly of western red cedar, but the CNC gave up in the middle and plunged a giant gouge right down the middle of my blade.  Another reason to switch to hand tools?  We have a new control board and everything seems to be back to normal.  I have also purchased the book Canoe Paddles: A Complete Guide to Making Your Own, and I would recommend it.