# Gear drawings for a 3 d printer



## Ron Frasier (May 6, 2020)

Doles anyone have some gear drawings for 16 dp,14.5pa with 5/8 bore I would like to try some printed gears for my 9 JR
Like a 52 t or80 t,64t.


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## devils4ever (May 6, 2020)

There's a gear tool in FreeCad. Type in the parameters and poof--it appears.


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## Ron Frasier (May 6, 2020)

where do i get this free cad


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## devils4ever (May 6, 2020)

FreeCAD: Your own 3D parametric modeler
					

FreeCAD, the open source 3D parametric modeler




					www.freecadweb.org


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## devils4ever (May 6, 2020)

Here's a 52T, 16DP, 14.5PA gear with 5/8" bore in FreeCAD (done quickly).


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## Ulma Doctor (May 7, 2020)

SOUTH BEND LATHE MODEL 9C ( 1937-1940 ) CHANGE GEARS  PART 2 by timbologist
					

This is the second part of a set of change gears for cutting threads on an 8TPI imperial leadscrew lathe these was designed for a South Bend lathe model 9C. The teeth have 14.5 degree  pressure angle The gear has a DP of 18 The module is 1.411 True involute form are  3/8" wide with a centre bore...




					www.thingiverse.com
				












						SOUTH BEND LATHE MODEL 9C ( 1937-1940 ) CHANGE GEARS  PART 1 by timbologist
					

This is the start of a set of change gears for cutting threads on an 8TPI imperial leadscrew lathe these was designed for a South Bend lathe model 9C. The teeth have 14.5 degree  pressure angle The gear has a DP of 18 The module is 1.411 True involute form are  3/8" wide with a centre bore of...




					www.thingiverse.com
				












						SOUTH BEND LATHE MODEL 9C ( 1937-1940 ) 127/100 METRIC TRANSLATION RING GEAR by timbologist
					

This is a Metric Translation gear for cutting metric threads on an imperial leadscrew lathe this was designed for a South Bend lathe model 9C. photo is of 80/63 translation gear as I don't think this 127/100 would fit my present set up need to make another banjo to make it fit. The teeth have...




					www.thingiverse.com


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## devils4ever (May 7, 2020)

Here's a step-by-step description on creating the gear above for reference. Since FreeCAD has a steep learning curve, I wish I had this when I was learning.

Creating a 52 Tooth, 16 DP, 14.5 PA Involute Gear with 5/8" Bore
----------------------------------------------------------------
 1. Start FreeCAD. See below to set preferences if FreeCad was never used
    before.
 2. Close Start Page (if desired) by clicking on "X" on tab.
 3. Click on "Create a new empty document" icon (top-left) or type CTRL-N.
 4. Select "Part Design" workbench from menu (top-center).
 5. Click on "Create Body" in Combo View->Tasks window (top-left).
 6. Click on "Create Sketch" in Combo View->Tasks->Start Body (top-left).
 7. Select "XY_Plane (Base plane)" in Combo View->Tasks->Select Feature
    (top-left).
 8. Click "OK".
 9. Create the bore of the gear by selecting the "Create a circle in the
    sketcher" (top-center). Icon looks like a circle with 2 red dots.
10. Move mouse to center of drawing area and click on center red dot (should
    turn yellow). Make sure the dot turns yellow. Otherwise, the circle will
    not be centered in the XY plane. Move mouse outwards and click again to
    create the circle.
11. Hit the ESC key to exit circle drawing mode.
12. To set the diameter of the circle, click the little arrow next to
    "Constrain an arc or a circle" (red circle with red line at about 1
    o'clock) icon select "Constrain diameter". Click on the circle just
    created and enter "5/8"" for diameter.
13. Hit "ESC" to exit circle constrain diameter mode.
14. Click on "Close" in the Combo View->Tasks (top-left) window.
15. Click on the "Model" tab in Combo View to see the Sketch just created.
16. Click on "Part Design->Involute Gear..." (top-left) to bring up gear
    tool.
17. Enter: Number of teeth: 52, Module: 1/16", Pressure angle: 14.5 deg.
    Leave High precision: True and External gear: True. Note that Module
    is the inverse of DP. Make sure you use inches.
18. Click "OK".
19. In Combo View->Model click on "InvoluteGear" (top-left).
20. Click on "Pad a selected sketch" icon (top-left). Icon looks like a box
    raised above a gray perimeter.
21. Enter the desired thickness of the gear in "Length". I used 1/2". Leave
    "Type" as Dimension. Leave others as defaults. Click OK.
22. The gear is 3D now but it cannot be seen unless you click on the
    "Isometeric" view from the top-right small box in the drawing area. Or,
    use the mouse to rotate the view as described below.
23. Rotate the gear to see the bottom. You should see a circle on the gear
    that is to become the bore. Select "Combo View->Model->Unnamed->Body->
    Sketch" (top-left). Or, select the circle on gear itself.
24. Click on "Create a pocket with the selected sketch" icon (top-left).
    Icon looks like a blue rectangle with a red center.
25. In the Combo View->Tasks window, select Type "Through all". Click on
    the "Reversed" checkbox. Click "OK".
26. Save the file in "File->Save As...". Enter a name under "File Name:".
27. At this point, the model is complete. I would use the "Path" workbench
    to create a G-code file for my milling machine. Since you are using a 3D
    printer, you would need to export the model to a slicer. I have no
    experience in this.

General Info
------------
 1. In the main drawing window, you can use the mouse to pan, zoom, rotate
    the drawing as follows:
    a. holding the center mouse button will allow you to pan.
    b. moving the center mouse wheel will zoom in and zoom out.
    c. hold the "Shift" key down, then hold the right mouse key down and
       move the mouse to rotate the 3D view.

Preferences
-----------
 1. Select "Edit->Preferences..." (top-left).
 2. Under "Units" tab, select "US customary (in/lb)".
 3. Select 4 for "Number of decimals".
 4. Click "OK".


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## Ron Frasier (May 7, 2020)

Thanks for all the work I have tried neuromas times and i just cant get it done i get stuck at number 19 and i don't know why .
I have a grandson who might be able to help me . thankls for all your help.


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## ericc (May 7, 2020)

Hey, this works.  Thanks devils4ever for those great instructions.  It took me several hours to work through this.  Freecad as included in the bionic beaver Ubuntu repository is broken.  If you type the error message into a google search, one of the first few hits says that this is a known bug and gives the correct solution, which is to enable the ppa archive to get the recent stable build.  Then, freecad comes up in a strange mode and requires a lot of fiddling to get to the workbench.  Then, dead in the water.  Searching on the error message on google again leads to a post to run the tutorial of that funny slanted part.  If you do this, it clears some junk mode that prevents working on the part body, and mysteriously all the steps work.  Oh, not the dimensions.  If you type in 1/16, it doesn't know what you are talking about, but 0.0625" works fine.  Also, the backspace key doesn't work in the text selection boxes, and you have to select with the mouse and overwrite.  Also, something is wrong with the mouse buttons, but fiddling works.  I am attaching the file created.  This is pretty neat, but as someone who has dabbled in software, this stuff is pretty sickening.

Oops, cannot attach file.  Unsupported type.  Well, it did eventually work, but you'll have to take my word for it.


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## devils4ever (May 8, 2020)

Ron: Sorry you couldn't get it to work. I've been playing and struggling with FreeCAD for some months now and I still get frustrated at times. I didn't even know there was a gear tool until about a week ago. Drafting software, especially 3D, is hard to learn. It took me a while to get used to this "parametric" drafting software. If you want, I can try and create a video of the steps.

ericc: Glad it worked for you. Wow, the install was bad? That would be challenging to say to least to figure out.

I started out using Fusion360 since FreeCAD seemed a littler harder to use and a little more limited. I switched when I perceived that Fusion360 was headed towards removing the free version for hobbyists. After using FreeCAD more, I realized they are both hard to learn and use and that FreeCAD is not as limited as I thought. I still have to look on youtube for videos on doing something specific. I found that google and youtube are your friends in learning FreeCAD since the documentation is lacking or obsolete. There's a lot of documentation out there that doesn't work because it's for older versions.


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## brino (May 8, 2020)

@devils4ever
Great guidance above! I did NOT know about FreeCAD.

@Ron Frasier
Another free option is Autodesk Fusion-360.
I wrote some about it here:
https://www.hobby-machinist.com/threads/gears-for-my-oldtimer-lathe.82245/post-718054
and here:
https://www.hobby-machinist.com/threads/gears-for-my-oldtimer-lathe.82245/post-718697

We both say "Free" but, as mentioned above, there is a cost of time to install, learn, and then finally produce the *.stl file.

-brino


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## RandyWilson (May 18, 2020)

There is more to "Free" than the price. Free of constraints and corporate overlords is of high value. Autodesk is within their rights to take the free version of Fusion the same direction as the free DNS hosting of Dyn, or the free photo hosting of Photobucket, or the free.....  FreeCAD can not be taken away from you.

 I spent a good chunk of my self-imposed quarantine learning FreeCAD, or rather making dump mistakes and getting frustrated at FreeCAD. Thanks so much for the gear pointer. Nothing I had read mentioned this lovely tool. Now to find some way to 3-D print a 9 1/4" 127/120 tooth gear.


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## ericc (May 19, 2020)

Freecad seems to suffer from some degree of lack of professionalism in the UI design.  They cavalierly render useless much good community produced instruction material by changing their UI in unpredictable ways.  Sometimes too much freedom is a negative thing.  I heard a presentation about this in which the example given was soccer without lines.  It would be quite a liberating experience, but most players would find the game more fun with the lines.

Sorry for the little rant.  You can probably sense that there are unhealed wounds.  One piece of advice:  it would probably be better to print a 127/100 gear.  This is far more of a standard size, and you can use all of the charts that others have produced.  Other good ratios are 80/63 and 47/37.  Having a 120 tooth gear may still be useful, but it is like a 22 tooth gear that came with my South Bend lathe when I bought it.  I puzzled over it for a long time before I figured out what it was for.


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## RandyWilson (May 19, 2020)

My understanding is they made some major changes to the UI design between 0.16 and 0.17. This was done to make things behave more to accepted industry norms.  Yes, it rendered instruction based on 0.16 obsolete, but that happens on occasion with everything. 

South Bend 14 1/2 and 16 use a 127/120 transposing gear set rather than 127/100 used on the smaller lathes. They also use a 6tpi lead screw rather than 8tpi, and a 24 tooth stud gear rather than the normal 20.  While some may see this as a gratuitous change to the UI (GRIN), it's how South Bend did it.  I already have the rest of the stock gearset, my lathe came with everything except the transposing gears and cover, I will do it the South Bend way.


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## brino (May 19, 2020)

ericc said:


> Freecad seems to suffer from some degree of lack of professionalism in the UI design.
> They cavalierly render useless much good community produced instruction material by changing their UI in unpredictable ways.



I am still suffering from the recent UI changes on Fusion-360!
They moved everything! 
It has set me way back; when I fire up the tool now I do NOT even recognize it, all the icons and menus have changed!!!

Many of the old youtubes are now less useful, including the Lars ones, as you cannot follow along step by step.
Some may argue that the short-cut keys may still be the same, but as a visual learner I learned the menus and icons. 
Now that's all gone!!! It is so frustrating!

Do I expect them to stagnate and not add features? No way, but just like microsoft adding those %!&!*($ "ribbons" to everything it is an unwelcome change inflicted on the user, with no thought for people like me.

I would love to see a "backwards compatibility" check box in the settings, to set the UI back to something recognizable!
It's the same reason I have add-ins for microsoft office to re-add the menus and am currently typing in Win7.

If I could buy the software for a reasonable amount, and then fully control (ie. disable) updates then I could guarantee the software tool would be the same every time I fire it up.

Perhaps I am just one of the old grumbly guys now.
Rant over......

I was the one suggesting Fusion-360 above, but maybe I need to get FreeCAD.........

-brino


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