A Pendulum Escapement Guide for 3d-printing

If you've ever seen one of those videos in which a youtuber makes some wild and crazy complex mechanisms, you've probably imagined how cool it would be to make one yourself. Which is why about a year ago, after seeing 1 or 2 videos of 3d printed pendulum clocks, I said "I guess it's finally time" so I got too it. Honestly, I failed once then gave up for a year, after that there were a lot of failures, but I didn't give up and made it in less than a month. The problem I had was most guides don't account for problems caused by 3d printing and how to fix it, that's why I'm making this.

With a proper guide, I imagine I could probably make this in a few days, it's not a hard task and I only struggled because I had a problem that I didn't understand and none of guides helped, I'll explain the modifications I had to make and the problems that caused them as I get there and also go through all the calibrations and how to make them.

For the most steps, I used a guide I found online from a big pdf (Headrick-EscMechanics.pdf (nawcc.org)) so they will be similar for a large portion but I'll give you the steps he gave with major modifications and personalization because his process will not work at base with 3d printing. Along with that at some point I split off completely

for this I will give you an image of the fusion sketch with measurements and some explanation.

I highly recommend going onto youtube and looking at a "deadbeat escapement" in motion, this will all make so much more sense.

all you need:

• a printer (I use a Prusa mini but it doesn't matter)
• PLA filament (or similar)
• a plastic water bottle or something to use as an adjustable weight
• CAD software (best if you use Fusion 360 as that's what I will reference)
• some string (I used a fishing line)
• some nuts/washers and a bolt OR anything that has some weight to it (somewhere around 0.5ib or 0.25kg)
• a measuring device (ruler, measuring tape, or dial/digital caliper)
• a meter long wooden dowel/stick that has a small diameter (mine is about .25in) you can find these on amazon or craft store, one meter length is important, diameter is unimportant

optional but useful:

• pegboard (this is to mount the test system but for now a table or just your hands will do)
• bearings (these are most likely unnecessary, but I prefer using them, I just went on amazon and bought a cheap 20 pack of bearings with an outer diameter of .75in or 19mm, inner diameter of .25in or 6mm, and a width of .25in or 6mm)

side note:

As I have only ever used a FLA printer, I am unaware how/if a resin printer will affect the process.

first off let's learn how to use parameters (skip to part 3 if you know it), if you aren't comfortable using parameters I'll try to teach as well as possible, if you still don't get it feel free to just skip this and I will have what to put if you don't use parameters for everything.

1. first, click on "display configuration table" in the configure tab.
2. next up, go click on the button in the corner of the table labeled "fx"
3. it will ask if you want to enter configuration mode, click yes.
4. a new menu should pop up, click the + button in the top right.
5. in this menu fill out the name with whatever you want I wrote "Size" this will function as a multiplier for the size so it is scalable but also so I don't have to do math for the non-Americans
6. with that said, enter "1in" or "2.54cm" (note that units are set in their own box)
7. repeat with 4-6 but name it "Angle_Offset1" and enter 3 for the equation.
8. make another variable labeled "Angle_Offset2" enter 40 for the equation.
9. make another variable labeled "Angle_Offset3" enter 49 for the equation.
10. make another variable labeled "Radius_Offset" enter .1 for the equation.
11. make sure to check the box labeled "configured" on each of them.

this will all be useful for adjusting later and scaling it (which I don't recommend going too small for)

1. create new sketch
2. make a circle at the origin
3. for the diameter enter "Size*5.87"
4. select construction linetype (first option in sketch pallete)
5. make a horizontal line going through the origin (make it about as long as in the picture but it isn't important)

if you didn't use parameters put choose either "5.87*1in" or "5.87*2.54cm"

for future reference the circle you made will be called "wheel circle"

Confused by the number 5.87?:

it's not actually the first circle drawn, it's the second, but since its all just a ratio and its easier to start there I chose to start there, the number it originated from is the 6 unit diameter arm wheel in the next step, this is a common pattern as the actual sizes are figured out with the lines in step 4 and 7, but those are at different angles to account for different things like expansion and such.

1. keep set to construction line
2. create 2 lines at a 45 degree angle from the horizontal to form a "V" length is again unimportant just make it a good bit longer than the circle
3. then make 4 lines offset by "Angle_Offset1*1 degree", look at picture for reference, length still unimportant
4. now change the offset of the upper left line to "2.4 degrees" (I don't remember why this worked as a fix but it's there)

1. draw a line vertical from the origin and for the length enter "4.243 * size"
2. at the open end of the line, add a circle with a diameter of "6*size" (this is the arm circle)
3. around the arm circle add two more circles
4. make the distance between the arm circle and each new circle be "Radius_Offset*Size" as shown in the image

in case you didn't catch it, the 6 unit circle is called "arm circle"

this step is where you begin to (at least temporarily) get more design freedom

1. make a circle in the center of the arm circle with a diameter of "0.5in" or "1.27cm"
2. now draw a line from the top of the new circle to the edge of the farthest arm circle, I drew it at an angle of 25 degrees from horizontal but anything below 35 degrees should work (you may need to draw a horizontal construction line as a reference for setting the angle)
3. make that line tangent to the small circle
4. now make another line going from the bottom of the small circle to the inner circle below the other line
5. now make the bottom line parallel to the top line
6. then make the distance between the lines equal to "0.25*size"
7. repeat 2-6 on the other side so that its mirrored

Notes:

the circle's size is done without the "Size" variable so it is always a constant size that is bigger than the axle which we will make later.

Notes for more creative designers:

The circle in step 1 can actually be bigger as long as it does not get too close to the wheel circle, also it could be a polygon or something, circle is just easier

also, the way I connected the two circles (the lines from 2-7) is mostly arbitrary, as long as there is enough clearance between that and the wheel circle it will be fine, once you understand the motion you can mess around with design a lot, but I would make sure you can make it work normally first.

we are going to draw more construction lines like the ones in step 4

1. make a construction line at 49 degrees from horizontal
2. make 2 construction lines offset by "Angle_Offset3*1 degree" from line in step one
3. mirror this on the other side

this is the most important part of the mechanism, its where the arm touches the wheel, almost all fine tuning happens here in the future.

for this I recommend really checking with the picture

1. on the left side intersection pictured above, make a line going from the top intersection of construction lines till it hits the furth construction line
2. set an angle of "Angle_Offset2 * 1deg" from the Constuction line that is only offset by 2.4 degrees
3. now on the right side intersection, draw a line going from the right intersection of construction lines till it hits the further construction line (not till it hits the other intersection)
4. set an angle of "Angle_Offset2 * 1deg" from the construction line as shown

1. only thing you need to do for this step is extrude the highlighted portion in the picture, pay attention to make sure the two sides aren't missing anything too
2. extrude a distance of "0.175*Size" (I know it's thin, but it not too important for strength)

YOU DID IT, THE BIG SCARY SKETCH IS DONE, this is about the 50% of the way mark, take a breathe and pat yourself on the back.

1. new sketch on the same plane as the last one (this sketch will be much less crazy)
2. project the wheel circle (5.87 diameter circle from the last sketch)
3. draw a new circle in the wheel circle with a diameter of "4.5*Size"
4. draw another circle in the circle with a diameter of "0.75*Size"
5. make a centered rectangle (the on where you place a center point and then the edge of the rectangle) center it on the origin and drag it to the edge of the smaller circle make the width "0.75*Size" and I cut the two smaller sides for simplicity

Notes for the lazy:

if you don't want to project it than just draw a new one and make sure it's the same diameter and position

Notes for the fancy:

the rectangle is just the simplest way to connect the two circles, you can actually do any design you want, swirly, stary, thin, three sided, four sided, whatever your heart desires.

important: as you make this make sure the tooth is leaning towards the vertical end of the arm

1. make a construction line to find the uppermost point of the 4.5 diameter circle
2. draw a line to the outer circle at an angle of 65 degrees from horizontal
3. use the center point arc tool (in Create>Arc tab) first click the center of the circles, then click the outer end of the line from step 2 and input "1 degree" for the measurement
4. draw a line from the end of the arc to the intersection of the first construction line made by the arc and the inner circle (if that's confusing use the picture as reference)

An unnecessary note from the writer about importance of the flat ends of the teeth:

all the guides online that I tried had sharp teeth ends, which is fine in wood/metalworking, but with a 3d printer, the software will actually cut out the end of the tooth because it can't do straight points (especially because they get infinitely thin at some point) this means the arm and wheel interact wrong and slip and caused me months of pain and confusion because I didn't realize it. In the end I found flat ends and a bigger diameter don't impact performance and reduce the problem to nothing, so that's the most important addition I added to the multiple century old process of making these that lets them 3d print easily. I must be fun to talk to I know (that was sarcasm).

1. select all the non-construction lines we made in step 11
2. use the circle pattern tool (in Create tab) and make the center point the center of the circles and for quantity enter "30"
3. now add a new circle with a diameter of "3.5*size"

1. select all the faces I select and extrude "1.75*Size"

that's it for the complex stuff, from here we will build a body for the mechanism, a pendulum, and test and make adjustments if needed

At this point my primary job is done, (kind of), if you can get the idea by reading through, then most of the stuff from now on is fluid and can be done by you in any combination of ways, but for those who need it, no worries, there's a lot more guide left.

1. create new sketch on the same plane as the others
2. project the arm and wheel circle so the center points are in this sketch
3. create a circle with a diameter of "Size*1" on both points
4. connect them with 2 lines on the left and right sides of the circles and make both ends of both lines tangent to the circles
5. make 2 circles in the other circles that have a diameter of "0.5*Size"

1. make an Inscribed polygon in both circles with a radius of "0.175*Size" and set sides to 3 (triangle)
2. set the bottom line of the triangle to horizontal (using the horizontal/vertical constraint tool)
3. now make a circle in both circles with a diameter of "0.475*Size"

1. Extrude the faces I have selected in the picture, note that I have only selected four faces, extrude them a length of "-0.25*Size" and select the "new body" option

1. hide the body and show the arm and wheel bodies along with the body sketch we just did
2. select the above shown face on both the top and bottom and extrude them "0.25*Size"
3. make sure they connect with the arm and wheel

1. create new sketch on the end of the axle on the arm (the end of the upper bit we just extruded)
2. create an inscribed polygon centered around the axle, with the sides set to 3 and the radius set to "(0.175*Size)-0.01" and set the bottom to be horizontal
3. create a centered square with sides "0.5*Size" by "0.5*Size"

instead of 0.01 as the constant being subtracted set it to whatever you want it to be so that it will slot in, give it space, 3d prints expand more than expected

1. select both faces and extrude "0.5*Size"
2. now select just the triangle and extrude "-0.25*Size"
3. now this is optional, but you can fillet the edges so that it bends to the side (which side doesn't matter)

1. create a sketch on the flat side of the piece and sketch a circle in the center with the diameter of the 1 meter wooden rod you are using for the pendulum (clearance is optional here because it's wood and if it fits snug than friction can hold it in instead of wasting glue)
2. create a second circle with a diameter of "0.35*Size"
3. extrude the ring out "1.5*Size"

there are other ways to make the pendulum rod than that, be creative, I came up with three or four printed designs that used a bad snap-fit joint before just using a wooden rod

Why one meter?

one meter happens to be (about) the length needed for a two second period meaning 2 seconds per tooth, this means the wheel will rotate once per minute, which makes it easier in the future. However, there are different lengths that count (pun intended) the equation is T=2(pi) * sqrt(L/g) where T=period (time), L=length (meters), and g=gravity (on earth that's 9.8m/s^2 so just enter 9.8 into the equation)

The bob is the weight at the end of the pendulum, this is vital because the length is actually the length from the center of mass to the point of rotation

Here's the thing, as everyone is going to have a different weight to attach to it, I won't walk you through my way directly, just remember that the actual weight doesn't matter as long as it can bring the center of mass to near the end of the pendulum

If you want to use it though, the way I did it was making a thing similar to the attachment piece but putting a threaded screw hole and screwing a small bolt that had heavy washers on it.

this is the part that attaches to the wheel

for this repeat step 17 but do it on the bottom axle

1. make a circle with a diameter of "1.5*Size" in the center
2. make a construction line from the middle to the top of the circle
3. make 2 lines from the center point horizontally out in opposite directions with a length of "0.3"
4. make a circle at both ends with a diameter of "0.2 * Size"
5. make a circle in the center with a diameter of "0.5 *Size"

1. select all of the faces except the two off-center holes and extrude it "0.05*Size"
2. now select everything inside the 0.5 diameter circle and extrude it out "0.3*Size" (make sure it joins with the other circle)
3. now repeat step 1 except extrude starting from the end of the last extrusion (select object from the start dropdown) and also only extrude a distance of "0.03*Size"
4. now extrude the inner triangle "-0.25*Size"

Printing can be done normally in whatever way you prefer.

To fit it all together, first put the axles on the arm and wheel side through the holes and then the matching pendulum and pulley through the triangle with some glue to make it stick, if they don't fit then sand the triangle till it does or reprint.

Thread the string through the holes and tie it down, make sure it can wrap easily around the pulley

now tie it around whatever driving weight, I find it's best to test with a plastic water bottle that is mostly empty and contains about 1/8th cup of water

The above picture is my failed attempts, of which you will have much less.

So you wound the pulley up, pushed the pendulum to go and it slipped or stopped before the weight hit the bottom

Well, that's going to happen most likely, if you expect to succeed magically on your first try, I have bad news, I might not, this is hard, but you got it.

how to adjust, the values in the configure tab should be a good start, play around with it and look at the motion of functional escapements then yours, I'm sorry I can't give you a master strategy, but every small detail can cause a change.

However, my biggest tip is to not just follow the traditional adjustments, try to change something and find the root cause but don't think it's one specific thing, getting caught on adjusting the arm cost me weeks of problems.

Remember for every minute you put in that satisfying "tick tock" sound is going to sound so much better.