Design and build of a mostly 3D printed watch

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jackfreecad
Posts: 53
Joined: Sun Oct 25, 2020 4:56 pm

Design and build of a mostly 3D printed watch

Post by jackfreecad »

I am in the process of making and building a 3D printed watch
It is based on a Roskopf Watch
The biography of G.F. Roskopf, the inventor and a descrition of the watch can be found in this free book here: http://www.watkinsr.id.au/buffat.html
And in french here: http://www.watkinsr.id.au/buffatFr.html
I use freeCAD 0.20, Part Design, Assembly4 and Gear workbench (Megagrand Fork)
It is still fairly big at this time, 144 mm in diameter and 90 mm thick
The escapement itself is five time the size of the watch in the book
All gears and frames are printed with a 0.4 mm nozzle on ender 3 in PLA +
Eventually, I will try to use a 0.2 mm nozzle and maybe even go down to 0.1mm and have real watch size parts
The arbors and steel pins are 1 and 2 mm piano wire
The driving gears are a module 1 cycloid profile
Winding gears are module 2, involute and bevel
Time gears are involute, module is 1.09
The power spring comes from a small engine recoil pull start, I might change for clock spring later on
The spiral spring is also 3D printed, it works for prototyping, but also experimenting with making one out of small piano wire and that is an adventure of its own right.
It does run, it can bee seen here:[url]https://youtu.be/KdQA8bHxzJo/[url]
More informations and files coming soon
Attached are pictures of the model, the first fully running prototype, and a view of gears
Attachments
watchGear3_4.jpg
watchGear3_4.jpg (146.78 KiB) Viewed 5612 times
protoFrontBack.png
protoFrontBack.png (856.17 KiB) Viewed 5612 times
ModelfrontBack.png
ModelfrontBack.png (455.84 KiB) Viewed 5612 times
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Shalmeneser
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Location: Fr

Re: Design and build of a mostly 3D printed watch

Post by Shalmeneser »

:o 8-)
jackfreecad
Posts: 53
Joined: Sun Oct 25, 2020 4:56 pm

Re: Design and build of a mostly 3D printed watch

Post by jackfreecad »

The project

Building an easy to build replica of a Roskopf watch with 3D printed parts
All the parts are 3D printed, the hardware and springs are steel
The spiral is made out of piano wire, patiently hand shaped
A 3D printed spiral is possible
The motor spring is repurposed from a small engine pull start
Quite big at this time, parts are printed with a 0.4 mm nozzle on a FDM printer
The size is 144 mm in diameter and 90 mm thick
Eventually I will redo the model in a smaller size using a 0.2mm nozzle
Then there is 0.1mm

Horology Resources

Books:
Links to books about the history of the original, including a detailed biography of G.F. Roskopf and a thorough study of his watch
The original In French:
http://www.watkinsr.id.au/buffatFr.html
In English and with additional graphics:
http://www.watkinsr.id.au/buffat.html

I have learned a lot about Horology with this book:
A Treatise on Modern Horology in Theory and Practice, Claudius Saunier
https://www.google.com/books/edition/...

Traité d'horlogerie moderne, Claudius Saunier
https://books.google.fr/books?id=vX1J...

Les Gravures en meilleures qualités
https://www.cliniquehorlogere.ch/fr/n

Book on hand making springs
http://www.watkinsr.id.au/blakey.html

Videos:
Part 3 of hand making a spiral spring
https://youtu.be/98wI6IA4TH0

Another video and another technique
https://youtu.be/Ebk1TzH6wUw

And my take:
https://youtu.be/612ysL7achE



Note:
My info:
OS: macOS Mojave (10.14)
Word size of FreeCAD: 64-bit
Version: 0.20.26238
Build type: Release
Python version: 3.9.7
Qt version: 5.12.9
Coin version: 4.0.0
OCC version: 7.5.3
Locale: C/Default (C)
Image

I consider myself still as a beginner with CAD in general and FreeCAD is the programm I am most familiar with.
I am a Mac user, so I favor the GUi approach whenever possible.Thank You to the comunity that make FreeCAD available on all platforms
I use Part Design, Assembly 4 and Gear Workbench
I did start with Fusion 360, then found the gear workbench in FreeCAD, from there I stuck with FreeCAD, now the 0.20 release. I switched to the Gear workbench ‘Megagrant” that offers more parameters to customize gears
I do not think FreeCAD is very complicate to use, or to learn, but it does take some dedication to get started, reading thru the forum and the user showcase is a good source of inspiration
YouTube has some good videos, make sure they are recent.
Learn about tological naming issues and how to avoid problems, it is not that big of a deal.
I will share how to avoid 99% of the issue and be aware of the remaining 1% and be ready for it
BTW, from my experience, Fusion 360 does crash and fail too!


WorkFlow

My process to design a watch or a clock
Design the escapement, print parts and test
Layout of the gears needed, starting with a sketch, it will become my Master Sketch
Using this sketch as a reference, make some disks and start a 3 D model
Plan for the needed frames, enclosure
Make a first assembly model, using my Master Sketch as a reference
Start importing parts in the model, always attaching LCS to dedicated sketches
Whenever a major change is needed, I start a new model from Scratch
Print and assemble parts, find new problems, fix, repeat!




Design of the escapement
Files for the escapement test attached

In Part design, I create a new document and a few bodies
In the first one, that use solely as a container, I create a sketch
I create several construction sketch following the instructions of the book
The original watch has pins of 0.2 mm, I decided to go with 1 mm pins for my 3D printed watch, all dimensions are time 5
Sketch 1, SketchEscapeAnchorPinSLayout, for the escape wheel and the anchor pins
Sketch 2, SketchAnchorBalance, is for the anchor to balance wheel interaction
Sketch 3, Sketch028LayoutGearV1, is a first potential layout for the gear and watch frame, more on that later

The escape wheel
I create a second body and rename it
I copy and paste/move the sketch 1 as a starting point
I reference that sketch to design the escape wheel
The fastest way is to do a disk, then cut one opening for the spokes, do a polar array
Reference sketch one to do one teeth, and again polar array to get 18 teeth

Tips:
Create the wheel at the origin, it will be easy to rotate it to study the interaction with the anchor
Right click on the body, go to appearance, move the slider to make the body semi-transparent

To avoid topology issues:
I create all sketches on the origin plane, in this case XY plane
With body being transparent, it is easy to do a new sketch and constraint it without hiding the body
Be aware that when using the sketch 1 as reference, the reference will break if you make change to it
Often time I do as follow
In a new sketch
Create the needed reference
Draw the new sketch
Delete the reference
Constraint the new sketch as needed
Pad or Pocket as needed
That way I can come back and edit a constraint with breaking anything
As an exemple: I edited the front angle of the teeth of the escape wheel to adjust the looking action of the anchor with escape wheel

The Anchor
I create a new body
I copy and paste/move the sketch 1 as a starting point
Create a new sketch
Using the origin as the pivot for the anchor, I reference sketch and draw the anchor
I create a new sketch for the Fork end and this simply extract dimension out of sketch 2
Often time, I will take a screenshot of a sketch of interest so I can view all the dimensions while I am working on sketch without going back and forth between two sketches
Once done with anchor, I use the transform tool to move the anchor where it belong
In this case 22 mm up
Now I can move the escape wheel and the anchor to study the interaction
For this I modify the angle
Select the body, click data, go to placement, angle
punch in an angle, or use the up down arrow
Do the same for the other body



The Balance wheel
A new body and a sketch, again at the origin for easy rotation
I use 2 pins at an adequate position for the interaction balance-anchor
The balance, for testing is of the gravity style, using a bolt in the hole to create a mini pendulum

The anchor V2
The anchor V2 was a later test with slightly off distance for the 2 pins, experimenting between locking face distance and impulse distance

Testing
There is 2 frames for the purpose of testing, Parts will rotate on 2 mm rods, with short 1 mm pins in the anchor and balance,
Testing is done against a wall or similar position
A string with a small weight 20 to 50 grams, attached to the escape wheel
Slow motion videos ia great tool to analyze the interaction of the moving parts
Test, analyze, edit as needed, repeat…

Once the escapement works as intended, time to design a watch around it
I duplicate the escapement document, clean out unneeded bodies, sketches, ect
And in the very first body, I started as new sketch, Sketch028LayoutGearV1
Time to experiment with various gear ratio, positions, source a spring, and about 500 sketch later, it is a estimate, have not counted, I have a watch

More to come…
Attachments
roskopfescapementStartV2.FCStd
(695.27 KiB) Downloaded 87 times
escapementTest.png
escapementTest.png (198.9 KiB) Viewed 5141 times
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JWorks
Posts: 18
Joined: Fri Mar 04, 2022 11:24 pm

Re: Design and build of a mostly 3D printed watch

Post by JWorks »

Hats off!

Great project and very well documented.

How long to get here?
jackfreecad
Posts: 53
Joined: Sun Oct 25, 2020 4:56 pm

Re: Design and build of a mostly 3D printed watch

Post by jackfreecad »

Gears

Gear ressources:

Cycloid gears for watches:
https://www.csparks.com/watchmaking/Cyc ... index.jxl/

Is cycloid gears obsolete?:
https://www.csparks.com/watchmaking/Cyc ... oen.xhtml/

More on Cycloid gears:
https://www.tec-science.com/category/me ... dal-gear//

Involute gears:
https://www.csparks.com/watchmaking/Cyc ... oen.xhtml/

Bevel gears:
https://www.sdp-si.com/resources/elemen ... #Section8/


The Roskopf watch

Specs from the book:
The spring has nine turns (for a nominal 36 hours of running)
The barrel rotates 1 turn in 4 hours
The barrel has 128 teeth, which for 17,280 vibrations, requires:
Second-wheel pinion 8 leaves.
Second-wheel 84 teeth,
Third-wheel pinion 7 leaves,
Third-wheel 60 teeth,
Escape-wheel pinion 6 leaves, and
Escape-wheel 18 teeth.
For 17,280 vibrations per hour, the ticking intervall is 0.2083 s
Gear ratio barrel to escape wheel:
8 x 7 x 6 / 128 x 84 x 60 = 336 / 645120 = 1/1920
To drive the hands, the barrel has a friction fitted gear and pinion
The barrel to minute hand ratio is 4/1 and th ebarrel to hour hand, a rational of ⅓
Those two combined give th e1/12 ratio between minute and hour
The time setting on the early version is done by hand, driving the minute hand


My 3D printed watch
The spring has 10 useful turns turns and the plan is get 12 hours of running time
The barrel rotates 1 turn in 1.2 hours
The barrel has 100 teeth, which for 9000 vibrations, requires:
Second-wheel pinion 12 leaves.
Second-wheel 60 teeth,
Third-wheel pinion 10 leaves,
Third-wheel 60 teeth,
Escape-wheel pinion 10 leaves, and
Escape-wheel 18 teeth.
For 9000 vibrations per hour, the ticking intervall is 0.4 s
Gear ratio barrel to escape wheel:
12x10 x 10 / 100 x 60 x 60 = 120 / 36000 = 1/300
To drive the hands, the barrel has a friction fitted gear of 18 teeth
The minute hand has a pinion of 15 teeth
The minute pinion drives the hour gear with a two stage 1/12 ratio
15/45 and 12/48

How did I get there?
Starting with the escapement:
With my running escapement, it looked like 0,4 s per beat would work
That is about half the original watch
It slower because of bigger parts that have more inertia, also slow means a smaller gear ratio between the barrel spring and the escapement
With a 0.4 sec/ beat with a 18 teeth escape wheel for an hour: (each beat, escape wheel move ½ tooth)
For 1 hour: 3600 / (0.4 x 36) = 250 rotation of the escape wheel
In 12 hours, I want 10 rotation of the barrel, or 1.2 hour for 1 barrel rotation
For one rotation of the barrel I need 300 rotation of the escape wheel: 250 x 1,2 = 300
The ratio of gears barrel to escape wheel will be: 1/300

Continuing with gears
One thing specific to horology is having a very slow motor driving fast moving parts
There is no constant motion, it all stop and go.
The efficiency of a big gear driving a small pinion is not very good
A pinion of 16 teeth is great, 12 works OK, 10 or 8 is possible
Watches do have a low as 6 teeth on low load high speed pinions
Historically, horology has used cycloid gears, Involute do seems to work just as well
I am experimenting with both
For the size:
I tried different modules I tried various combination and found that I could do nice cycloid profile pinion
with a module 1 using a 0.4 nozzle, since the width of the leave was 0.83 mm
The barrel for the spring worked well with a diameter of 96 mm
And that is how I came with 100 teeth for the barrel gear
The minimum size that I wanted for the pinion was 10, and 12 for the first stage, after playing around with numbers I ended up with 100/12 x 60/10 x 60/10
With the barrel meshing the second gear 12 teeth for the pinion and 60 teeth for the gear, this set up the dimension of the frame:
With a diameter of 100 for the barrel gear meshing the 12 teeth pinion connected to a 60 teeth gear
Max size when factoring the head dimension: 100 + 6 + 30 = 136 mm
And that fits in the 144 mm frame of my watch

Main Sketch

Check out the mainSketch: barrel to escapement and winding gears
This sketch is the foundation of the watch
At this time, no change can be made to it
If working as a team, this sketch should be locked.
This sketch is a reference for many parts of the watch, it is also a reference for the Assembly model
I know that if I make changes here, many issues will be happening and that is NOT a topological issue
It is probably possible to make it fully parametric and based on a spreadsheet, but I have not tried that.
If I really want to make changes, then it is time to start a new project
I have started 6 times, this model is number 6

Model for gears testing

Attached is an Assembly 4 model with two cycloid gears, 60 and 10
Click on the 2 gears in the menu, or: Assembly, Animate Assembly, select variable move, set range 0 to 111, run.
The sketch1 in the model sets the position of the gears, the LCS are attached to the circles at the end of the line
More to come…
Attachments
gear10cycloid-60animate.FCStd
(794.42 KiB) Downloaded 72 times
mainSketch.png
mainSketch.png (288.35 KiB) Viewed 4872 times
User avatar
Shalmeneser
Veteran
Posts: 9475
Joined: Wed Dec 23, 2020 12:04 am
Location: Fr

Re: Design and build of a mostly 3D printed watch

Post by Shalmeneser »

You should compete to <0.20 splash screen contest> (https://forum.freecadweb.org/viewtopic.php?f=8&t=66492).

Complex main sketch.
jackfreecad
Posts: 53
Joined: Sun Oct 25, 2020 4:56 pm

Re: Design and build of a mostly 3D printed watch

Post by jackfreecad »

I am getting to a point where I am going to stop on this project and share it with the following licence:
http://creativecommons.org/licenses/by-nc-sa/4.0/
Get the full file here:(I think, be aware 39MB)
https://drive.google.com/uc?export=down ... QDNAJHJYzX

FreeCAD is full of gems!
FreeCAD has a very simple way to share your 3D CAD model with non CAD people, just 2 steps:
Check it out below, spin and zoom as you wish, works on mobile too:
watch8.png
watch8.png (406.12 KiB) Viewed 3584 times
https://jacprog.github.io/roskopf3Dmodel/watch8.xhtml
I had been looking for a way to present a 3D model of clocks that I have made and searched how to produce a 3D PDF.
There is way with asymptote and latex and while searching the forum, I came across this solution in this thread:
https://forum.freecad.org/viewtopic.php ... ec3389c6d8
I looked into latex and got lost along the way, however at the end of this, thanks to wmayer and easy-fc, there is a great 2 step solution
Export the model as .step
Import the .step and export as .xhtml
The result is a file that can be shared and opened in most web browser, no CAD program needed
And with the proper code, it can be served from a webpage such as this example too:
https://easyw.github.io/FC-videos/3d-html.xhtml
My point here is that the forum is a great source of inspiration and knowledge
The users showcase has some great examples of what and how FreeCAD can be used
Thanks to ppemawm and others who show case their designs in the forum
And these days, using the search feature in the forum is my main source of knowledge
So my take on FreeCAD after about a year and a half of use:
FreeCAD is a great CAD program
FreeCAD is not that hard, sure there is some learning to do, and I probably know less than 10% of it, or maybe between 1 % and 10 %
In order of knowledge:
Sketcher
Part design
Gear workbench
Assembly 4 workbench
fastener workbench
NOTE:
I am a MAC user, so mouse and GUI is my way. For me, the keyboard is just for text and numbers...pretty much
I am not an engineer, just a maker and tinkerer
I did have some formal training with AutoCAD, then used Fusion 360 for a while
I have been drawing stuff on paper for over 50 years
For me the best way to learn is to have a project
Then it is to find a way to use the tool I have to produce the result I want
For me, the topological naming issue is not a big deal
Everything that can be based on a sketch can be rock solid, chamfers and filets, just do them last!
My workflow:
For the frames:
It starts with one or more sketches to locate all features, location of gears and arbors, etc...
Then using those sketches as references, I create new sketches in the body to create pads and pockets
The vast majority of sketches(99%) are located on primary plane XY, XZ or YZ, I could offset them but I do not, I prefer to use the two dimensions to do extrudes and pockets where I want them to be
Whenever I need a datum plane, I will attach it to a reference sketch, rather than to the body
Sketch is steady, body can change
I also set the apparences of body to 40 to 50 % transparency so I can see the sketch as I go to build and edit them
While I use Assembly 4 to put all parts togheter, I usually start by making the part in a separate document. It is easy enough to just copy and paste to import new parts in the assembly document
I usually create a specific sketch in the body to attach the LCS, that way if I edit the part, the LCS stay tied to the sketch rather than to an edge of part that will surely move around
In the assembly, I will also use a sketch to locate all LCS, and if need to add to the sketch, I would rather make a new sketch to add new LCS to the assembly, this again to prevent topological issues
A few issues I have with freeCAD, some might be the way I use it
High number of patterns can slow down the system
When doing gears, I have done gears up to 120 teeth, then adding some features and edits to the 120 teeth can slow down the system
Threaded rods with two flat sides, so they can be 3D printed flat on the bed is a challenge for FreeCAD
threadedrod M10x 65 flats.png
threadedrod M10x 65 flats.png (139.84 KiB) Viewed 3584 times
file is here: 1.4 MB
https://drive.google.com/uc?export=down ... JLDI89Ub9x
I make a M10 X 65 threaded rod using the fastener work bench
I cut off two flat side so I can print it flat on a bed
I make a clone to reduce the diameter to 96 % to allow for some clearence
This takes 2 to 4 minutes to generate
Maybe there is a better way, I would be glad to learn
Needless to say, I do not include those parts in an assembly
OK, now no offense, I have tried hard too look in the weakest point of FreeCAD, it is still great a great software
Thank you so much to all of you that have put so much effort to make FreeCAD such a great CAD software
I will be back with more projects
BTW
I got a new computer, as user, it just works!

Code: Select all

OS: macOS 10.16 on M1 MacBookPro
Word size of FreeCAD: 64-bit
Version: 0.21.29485 (Git)
Build type: Release
Branch: master
Hash: a236ca843fdd6674afb6d7ed1454fbd3b547f5ea
Python 3.10.5, Qt 5.12.9, Coin 4.0.0, Vtk 9.1.0, OCC 7.5.3
Locale: C/Default (C)
Installed mods: 
  * freecad.gears-megagrants
  * fasteners 0.3.40
  * Assembly4 0.11.12
I also got my second back up 2007 Mac Book Pro with POP OS to run FreeCAD 0.20 just fine
jackfreecad
Posts: 53
Joined: Sun Oct 25, 2020 4:56 pm

Re: Design and build of a mostly 3D printed watch

Post by jackfreecad »

I realize the sharing of files was incomplete
link to frames assembly: watch8Frames
https://drive.google.com/uc?export=down ... gvPYWepPwr
link to gears and mobile parts with the frames nested in: watch8CycloFinal
https://drive.google.com/uc?export=down ... uSbGecYvKk
download both files
put them both in the same folder
Open: watch8CycloFinal
in FreeCAD

Note:
Viewing gears should be fine
If editing gears, it might cause some error!
The gear workbench have had some changes lately and the newest option might not be compatible
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