Creating the 12O'Clock calibration level in FreeCAD

[c0depr1sm]

In response to that post, @BradM created a nice tool to calibrate the Malsow 12 O’Clock chain positions.

I designed a CNC version of it. Here you’ll find a description of how I made that with FreeCAD.

If you would like to follow-up, you should get the free open source FreeCAD tool version 0.18 or later. (As of january 2019, do not the CONDA flavor as some bug disables tag generation).

Then download the 12OClockLevel FreeCAD project distributed here under a free and open source GPLV3 licence.

Step 1

Took a contrasting picture of the gearbox sprocket, using my camera with some close-up ( macro) focus capability.

Step2

Imported into free and open source Inkscape. Used menu “Path/Trace Bitmap” to convert the bitmap into a vector shape. Then ungroup the set of shapes, keep a good one showing at least part of the sprocket profile. Edited the shape (cut nodes to isolate one good teeth, Path/simplify to reduce number of nodes for same shape, and duplicate / rotate 10 times at 36 degree) to rebuild a full sprocket profile shape (right click and download the shape to get the actual SVG shape file).

Note: use color fill, no contour on the inkscape shapes. This makes FreeCAD importation more accurate.

Step 3

Tried to make a shape that can be CNC with a 3.17mm (1/8th inch) router bit… But should have kept it like that.

Step 4

Setup the inkscape file properties to use mm units, scale the sprocket shape to be like the real one. Having a caliper here is quite necessary.

Step 5

Added a rectangle above the sprocket shape to position the level vial cutout. Now, FreeCAD will let you tune the shape later if you want. But to get a good fit later: a caliper.

Step 6

Combined a copy of the vial level cutout and sprocket shapes (path/combine) and used the menu “path/dynamic offset” to create shape that can be swelled using a handle. Swelled until made them touch to overlap. Used path/union to create a single closed shape. Then “path/brake apart” to get rid of all little artefacts like holes. Selected the swelled contour only. Cleaned-up nodes to give the contour the desired V shape surrounding nicely the sprocket and level vial.

Step 7

Added a circle in the sprocket shape center, then align everything using menu object/align and distribute. Make sure each shape is closed (has a fill color).

Step 8

Saved SVG file as a plain .svg file – NOT inkscape .svg file

Here is a file showing the result (again the sprocket shape was overkill here)

Step 9

Opened FreeCAD, created new project, open part workbench and created a new part.

Step 10

File/import selected .svg file and chose import as geometry when prompted. At that point got a set of shapes. Not yet sketches.

Step 11

Opened the draft workbench. For each shape, menu “draft/Draft to Sketch” once with each shape selected to create a set of equivalent sketches. From that point only use the sketches.

Step 12

Used Sketcher workbench to edit sketches to clean them up: (I did not fully constrain the sketches. I kept closed loop sketches)

1. Replaced the circle with a real circle: The inkscape import created a B spline and that is not supported by all path generation tools. Especially not the Helix which I wanted to use.
2. replaced the level vial slot with a real rectangle

Actually, B-Splines are complicated shapes and the Path Workbench will slow down if you get too much of those. That is why I prefer to use sketches with FreeCAD shapes instead of inkscape. But here the sprocket was definitely worth the svg import!

Step 13

Used part work bench to extrude the contour sketch, then the part design workbench to pocket holes partly or completely using other sketches.

Step 14

When trying to make CNC paths, found out that the sprocket tips needed to be cleared, but a 3.17 mm bit can’t go in. Added a set of 10 circles pocket with polar pattern to drill the tip of the sprocket teeth.

Step 15

Once the part was defined, opened the Path workbench to create a path CNC job, operations and simulate stock machining, then exported GCode.

I invite you to inspect how the 12OClockLevel FreeCAD project is built.

To learn more about Path workbench, I strongly recommend Sliptonic’s youtube tutorials. I don’t get benefits for that recommendation. But I got all my FreeCAD and Path workbench starter skills with it

Step 16

Inspected GCode with CAMotics and looked good. But later found that G81 (drilling) is not suported. And had to replace the GCode lines with equivalent sequence:

G81 X16.2196 Y16.1716 Z-9.0000 F300.00 R10.0000

becomes

G0 Z1.0000
G0 X16.2196 Y16.1716
G1 Z-9.0000 F300.00
G0 Z1.0000

Where the R10 retract is simplified to pull the drill up to 1mm instead given the MaslowCNC nature.

Here is a reference for GCODE commands at LinuxCNC

Step 17

Then I had to tune the fit. Again with a caliper I could see that my cutter was cutting 0.15mm too close when profiling. So I mofified my tool in FreeCAD to set it 0.3 mm diameter bigger (3.5mm) and that actually made the path get further away from the profile faces. My cuts were then snugly tight.

Note that to effectively modify a tool in a CNC job, you have to double click on the tool controler of the CNC job, then look at the end of the settings panel to see the TOOL tab, expand it and change the tool diameter there. If you change it in the tools manager, the change will have no effect unless you delete and recreate a new tool controler for the job.

And that is it.
Let me know if you try FreeCAD projects on MaslowCNC!

[Gero]

The reason why this is not cut out (until now) in acrylic today is https://youtu.be/Cx2Iep_lXWQAny advice if i have to scrap my attempt or can draw new lines and proceed?

edit: i forgot the most important!
A huge ’ standing ovation THANK YOU’ for this detailed write-up of open-source and free workflow!

[c0depr1sm]

Now that level vial response is not what one would expect!
I salvaged mine from a unused tool. So I can’t recommend a source.

However, When reviewing specifications of a vial manufacturer/distributor, here is what one finds: Sensitivity ranges from of 31’ to 62’ per 2mm displacement.

If I understanding it right, this means a 2mm lateral displacement of the bubble in this case amounts from 31 to 62 minutes of a degree. That is 0.5 to 1 degree for 2mm.

According to the analysis presented above in the first post of the current topic, that is dividing the 3degree example error by 3 to 6. Thus causing a 0.25mm to 0.5mm center drop or lift on the top edge center.

Now is that a small error? At least now we can estimate it!

Anyway, all that is if you vial is behaving within that specification. And that is uncertain because normally, a vial would be balanced.

[BradM]

I used a different method to get the sprocket shape for the 3D printed version. I think your way is more accurate, but I just wanted to mention this other method in case anybody is interested.

I downloaded the 2-D DXF drawing from McMaster-Carr here.
Then I converted it to SVG using an online converter tool, then used Inkscape to delete the extra parts of the drawing that I didn’t need as well as cleanup the paths of the gear.
Then converted back to a DXF using the online converter so that I could import it to Onshape.

If anybody is interested here is the Onshape document for the 3D printed version: https://cad.onshape.com/documents/7aa2f8c5357e5001dad22c33/w/de7b178aecedfa8adf013ffd/e/a87334a5393d9daab70d59b0

[Gero]

Finaly!
0.17 and 0.18 crashed on me when trying to import a .sgv as geometry
I ended up spending nights to design the sprocket from scratch. Learned allot in FreeCAD though.

[c0depr1sm]

Wow!
I like the “full visibility” concept!
Very neat.

How do you work … (acrylic?) tools, etc?

@Gero

About crashing .svg loads… Did you use a svg file in inkscape flavor?

@c0depr1sm

Step 8

Saved SVG file as a plain .svg file – NOT inkscape .svg file

[Gero]

I tried both, the plain first. I tried 3 days in a row and changed from 0.18 ‘something core bug’ to an other.
Also had several attempts to change the thickness and sketches in your file

[Gero]

@c0depr1sm

How do you work … (acrylic?) tools, etc?

A cheap old china desktop cnc 6040z bought second hand and never serviced (parallel port ).
8 mm acrylic (real life 7.8) cuts 7.8 mm on this machine if i design it at 8mm. I researched acrylic feedrates from several sources and found within 1 test that going a little lower on the feed (metric F1800) and not half of the 1/8 " (3.175mm) what would be 1.5875mm to 1.2mm with a 2 flute upcut bit looked just perfect.
Edit: FreeCAD → linuxCNC
Edit2: From the research i remember that there was a big difference in acrylic. Something like moulded or other? Will try to look it up. I had no melting, so i got the better one that is not the one from the chaep markets.