Need advice on the calculations for cutting a semi-circle on the XZ axis

[tooold]

I am trying to cut a semi-circle slot 3/16 in diameter but Mach3 does not support cutter compensation on the Z axis. I believe the only way this can be accomplished is by coding the X and Z movements. Is there a formula, set of calculations, online g-code generator(haven't found one) which will plot the points? Any help would be appreciated. attempting to

Similar Threads:

• Design calculations for a cutting wheel
• Cutting Force Calculations
• Inertia Calculations - Cutting Speed & acceleration
• Cutting Load Calculations
• Semi-newbie looking for some design advice

[Jim Dawson]

I'm a little confused, I'm not sure what cutter comp has to do with the Z axis. You should be able to input a tool height offset value if needed.

Having said that, what you are really wanting is a G18, XZ arc move. Your CAM program should be able to generate that and output the proper G code.

[murrayadams]

im not sure if im understanding the problem correctly. but i think had to do something similar. i had to cut half a scotch key into a new hydraulic rod to suit an old piston.did it with a ball end milling cutter smaller than the desired size used small stepovers. this was with the help of a cam program and a cnc. if you dont have these you need a tool of the correct profile.

[tooold]

After reading my post I realized that the information was very skimpy. Retake.

I am trying to cut a series of slots 1 behind the other viewed from the Y axis. The slot (semi-circle) is on the X axis and should be .187 in length. Using a 3/32 ball nose. The problem is my slots are too wide (.264) if I issue something to the effect of G18, G02 X.187 R.09375. Depth is OK , but this is not a semi-circle. If I shorten the X value, the the R value will have to be shortened to no more than 1/2 of that value because Mach3 will simply ignore any R value greater than that. It would simply move the cutter X distance. i.e. no Z movement. Likewise, if I use the I Z format of the G02,03 command it gets upset if the points are not of equal distance.

I can't spell CAD. Have downloaded FreeCAD and CAMBAM but as yet haven't figured out how to use either. Work in progress. It occurred to me that the authors of these products have to plot cutting points so I assumed that there must be some mathematical way to do it myself. Am I all wet?

[Jim Dawson]

About 4 years ago I couldn't spell CNC either and I'm 67, so there is hope I have never used FreeCAD, but have been using CamBam for a few years. I'm no expert in Mach3 either, but G code is G code.

The points are calculated using trig. Here is a pretty good write up https://en.wikipedia.org/wiki/Atan2 and a calculator https://www.easycalculation.com/trig...calculator.php

Please provide a drawing or picture of what you are trying to do, I'm having trouble getting my head around it. Any rough sketch on a piece of paper will do.

[ger21]

He's cutting an arc in the XZ plane, and because the center of the tool is following the path, the cut is actually elliptical, rather than circular.

[Kiwi]

What about this?
Touch tool on top of plate and set as Z0.0469
G01 X-0.0469 Z0.0469
G01 Z0
G18 G02 X0.0469 R0.0469
G01 Z0.0469
G00 Z1

[tooold]

Wanted to take the time to thank you guys for your help.

ger21 - you summed up the problem in 1 sentence. Ah, you real CNCers with real equipment!

Murray - the tool profile. I tried with a 3/16 cutter. Plunged 3/32 deep. Moved Y axis forward 3/32 and plunged again (kept repeating for 5/8 up Y). Moving the cutter 1/2 it's diameter forward leaves a raised band between the cuts where they became tangent to one another. Think the little segments on a fishing worm. I may have to go with this. However the segments were too wide so moved to 3/32 cutter and began trying the semicircles.

Jim - read your links. It threw me off on a tangent such that I coded a script to compute the points on the profile and generate the gcode. It produced exactly the same cut as the G18 G02 I had tried
so I knew I was closer, because I could throw in a few adjustments as is were. By the way, I am older than you and have a fraction of your experience. I was looking at my join date and realized that it had taken me 8 years to finally decide to convert the little mini-mill to CNC. Would have liked to convert the Acer but don't have the coins. If you're interested try this link
http://www.wseas.us/e-library/confer...S/SEPADS08.pdf
good stuff but it's upside down and backwards. If I can just figure out how to determine the "profile slope line", in figure 4, I could hurt him.

Kiwi - when I got on the net this morning and saw your reply I immediately wrote it down, took it out to the shop and tried it. Looks good. Width is good. Depth is questionable primarily because
1) - I may not have followed your instructions properly
2) - This is a home built machine and to lose 3 or 4 thou is normal
3) - Only method I have to measure the depth is very crude at best

the depth was .059, about .034 shallow. This may have been due to my set up. Am I correct in assuming that you wanted the cutter touching the surface but the DRO reading .0469? The first line of code was G01 X-0.0469 Z0.0469, no Z movement.
More testing forthcoming.


I'm through mouthing now. Again thanks

[Kiwi]

Am I correct in assuming that you wanted the cutter touching the surface but the DRO reading .0469?

Yes That's correct

The first line of code was G01 X-0.0469 Z0.0469, no Z movement.

That line moves the cutter to start point

I'm not sure if the arc is G02 or G03

Suggest you try doing the arc in two moves. (see below)

G01 X-0.0469 Z0.0469
G01 Z0
G18 G02 X0 R0.0469
G18 G02 X0.0469 R0.0469
G01 Z0.0469
G00 Z1

[tooold]

Kiwi,
Good and Good. Came within 3 thou of being perfect and that ain't bad for a cobbled up $300 machine. After many cuts I decided to go with the single cut as it seemed to produce a smoother cut.
Again, thanks