I was trying to avoid using the MultiCam since I haven’t been able to take the class yet, but I’ve exhausted all other options so here I am, pleading for help! All I need is a 14" diameter circle with a 2.5" x 2.5" pocket in the middle (.65" deep) cut from some walnut I have ready. I was hoping to just do it on the Shapeoko but it’s just too big and I don’t trust myself to cut a half decent circle by hand.
Anyone willing to help out?? I got a 6-pack with your name on it if you are!
The pocket is also a circle? Concentric?
The stock is how thick?
Is one side reasonably flat / smooth?
The pocket is a square, 2.5" by 2.5" in the middle of the circle. It’s a clock face, so that’s where the mechanism is going to go, and I’ll ultimately drill a hole in the very center for the shaft to go through. The stock is about 16" by 16" square that’s 0.81" thick. It’s all flat (I squared it up before gluing together).
Do you need the corners over-cut to fit sharp corners on the mechanism?
Why not drill the center hole with the router while you are at it? That way it is perfectly centered to the outer perimeter and the square cutout.
Not sure what you mean by over-cut (showing my lack of knowledge here) but the actual mechanism is a 2.25". Really the pocket could be 3x3 with rounded edges, doesn’t really matter since it will be on the back
Here is an example of over-cut:
Since the CNC router uses a spinning bit, it cannot produce an interior sharp corner. If you route a pocket using a 1/2" diameter bit then you get corners with a 1/4" curve. A 2-1/2" pocket could accept a square object that is only ~2.34" square (left illustration). If you want a 2-1/2" pocket that can accept a 2-1/2" square, then to route the sides past the edge (right illustration) to create enough room.
That was great explanation and illustration, thanks!! Makes perfect sense. On this particular piece no over-cut will be needed since it’s not necessary for the piece to fit in that snugly. And yes the center hole could be cut with the MultiCam as well, I was just trying to simplify as much as possible since I’m asking for someones time.
Diameter?
5/16" diameter.
character limit
Just so you know, if you add something V-carved (e.g. signature on the back) you would have enough to check-out on the MultiCam. (You would also have to take the class.)
I have the model made. I’ll post some files later tonight.
Except for having taken the class, which teaches the other important basics of CNC routing.
Should the center be the reference or a corner?
Before answering consider carefully how you want the exact center of the clock to look and whether or not you want reusable leftovers.
I would say the center be the reference… the piece is actually 3 boards joined up so I’d like the center of the clocke face to be in the middle of the middle board, if that makes sense. Plus I’m not overly concerned about the leftovers. Let me know if I’m thinking about this wrong.
Thanks so much for all your help!
Yeah I’ve been trying to get into the class, they don’t happen too often and fill up quickly, but I’ve been checking daily for the past few weeks so hopefully I’ll get in the next one!
Sounds good to me.
This should give you an idea of the difference…
Start cutting from the lower-left…
Start cutting from the center…
Clock Face.zip (270.4 KB)
…should contain a SolidWorks model, a DXF file, an STL file, and the VCarve file. There are four tool changes. The machine time is estimated to be ~12 minutes. The CNC files (with an instruction sheet) are in the usual place under roughvagabond\Clock Face.
The 1/8" endmill (Onsrud 52-240) has a cutting edge length (CEL) of 0.50 in. Rather than take any chances, this version removes two toolpaths that may have been troubled by a CEL less than the stock depth. The CNC files have been updated.
Clock Face.zip (246.6 KB)
Huh. We have an upcut 1/4" endmill and a need for an upcut. I may have to make one more version…
The cutting edge length less than the stock depth makes sense as a possible issue. What is an upcut needed for? Is that because the face of the piece will actually be on the bottom? I just don’t know what all the bits do and when to use them.
Thanks for all your help on this Brian!
Correct. It should give a nice clean sharp edge for the clock face (which is the bottom when on the MultiCam).
In my experience the differences are best described as “helpful”. If you use the “wrong” endmill you can still easily end up with good results. “Sharp” and “free of defects” are far more important.
A downcut endmill gives a nice sharp edge on the top of the stock and helps hold the stock down. The disadvantage is that the chips are not naturally cleared away. Accumulated chips can cause problems like knocking the stock free from the vacuum hold-down, overheating the endmill, or even breaking the endmill. But, those problems are easily avoided if the chip collection vacuum is working well or if cuts are done so the chips fall away.
An upcut endmill gives a nice sharp edge on the bottom of the stock and naturally clears chips away but tends to lift the stock from the table.
I no longer use compression endmills. At the bottom they are an upcut. At the top they are a downcut. The idea is to get the advantages of both.
I believe the V-bits are all upcut. Their purpose is simple: cut an angled edge. They can be used to make a bevel or decorative lettering or anything else with a simple angled edge.
I tend to use 1/4" and 1/8" endmills. The linear speed is not much faster for 3/8" endmills (216 vs 252), I have had 3/8" endmills knock stock free from the vacuum hold-down, they seem to get abused more (chipped, dull), and there is more waste. In contrast, I have always been able to find razor sharp 1/4" and 1/8" endmills in the drawer. I tend to use 1/4" to “rough” (even though the result is usually between “very good” and “excellent”) and 1/8" to “cleanup”.
In your case, the 1/8" is necessary to mill the hole for the shaft. I originally had a cleanup pass with a 1/8" endmill but eliminated it out of concern for the cutting edge length. The 1/8" could also have been used to reduce the radius on the pocket for the clock mechanism but the depth also exceeds the cutting edge length.
Make sense?
