What's new
What's new

Dialog 4 programming exercise

Did you hear about the guy who built a wooden car, wooden block, wooden pistons basically everything wood. Wooden go.

Nice job. Be careful of what wood you cut, I machined a pistol grip from some mystery wood on a Deckel 60T and the table rusted everywhere the wood touched.
 
Did you hear about the guy who built a wooden car, wooden block, wooden pistons basically everything wood. Wooden go.

Nice job. Be careful of what wood you cut, I machined a pistol grip from some mystery wood on a Deckel 60T and the table rusted everywhere the wood touched.

Yikes, that stinks. I had a Shop-Vac going the whole time it was cutting.
 
To do that on a 3 axis you would need surfacing, with a ball end mill, with the radius that is at the bottom of that cylinder intersection
dunno if their is any canned cycle that can do that from my convo programming days on even newer machines.

1714656702737.png
 
I have done arc features like that using a ball endmill in the vertical spindle and G02/G03 arc moves in the G18 or G19 planes. The hard part is wrapping my head around tool length comp and the location of the arc center. It is similar mental effort to putting a lathe tool in a vice and work in an ER collet to make a CNC lathe. Everything seems bass-ackwards.
 
So the next question is, how would you guys go about programming for this radius? Would anyone attempt this without CAM?

I think I could fingercam that for a vmc in about an hour for a 1/8 ballmill and .02 stepover which would leave little ribs in the finish but for what it does it would be fine I'm sure. About half the time to draw and program it in my cadcam with a .005 stepover leaving a pretty smooth finish. I fingercam quite a few of my little projects like this just to keep the skills that I struggled to learn as a kid when we didn't have anything more than paper and a calculator with a bunch of extra buttons.
 
You may remember this from somewhere, it was all fingercam from conception to install.
View attachment 438222View attachment 438223View attachment 438224

Yes, of course. Even the clamp bracket was fingercammed? Nice. I am going to take a crack at my part and see what I can come up with. I'm pretty good with math, trig and such. Mostly because, like you, I prefer to use it once in a while and keep it fresh in my memory.

The tricky bit is going to be going around the boss/pin. My machine doesn't have simultaneous 3 axis helical type movement as I understand it, except for certain specific canned cycles, so anywhere I run into the boss I'll have to stop and rapid back then move to the next pass rather than go around. I'm thinking if I program the one side that would collide with the pin, I can mirror the other. Anywhere that doesn't hit the pin should be easy.
 
Even the clamp, I cut the profile with a 1/2" endmill then followed with a corner rounding router bits with a 1/2' minor dia so the numbers are the same for all 3 cutters keeping all the cutting 2d. I think keeping the math alive is good for your head but the cad cam is how I do most of my "work" and fingercam my own projects.
You could cut your arc up to the boss, move out and up in z, sideways to the boss and arc back down as you move away and avoid all the little rapid moves.
 
Here is a part where I had to use the G19 and ball endmill/vertical spindle trick, to form the half-round sparkplug passage between the fins an not hit the boss protruding above. There were hours of gears screaming away at 6300 RPM with a 1/16" ball endmill. I think I made 14 or 16 of these, two at a time using Deckel's version of multiple work offsets (G54, G55) This was probably the peak of my finger-CAM abilities, and I am not sure I could repeat it.
DSC00020 (1).jpgDSC00015 (1).JPG
 
Don't overlook G9 G03. If you use polar coordinates, then the only points you need to worry about are the centers of rotation. So it is easy to do circular contour on Deckel, as long as you do your own cutter comp to get the start point set correctly. i.e. you have to move the center of the ¼" ball mill, not the bottom of the cutter... You can go back and forth from XY to XZ (or YZ).

I'm in a hotel room so I can't look up the full syntax of the G9 command, so there is little hand waving here.

e.g. changing the problem to machining a corner radius on a 2" dia. cylinder. I,J and K are absolute coordinates.

N1 G1 X0.875 Y0 Z.125 <- Set Z0.125 when the ball mill touches off
N2 G9 G3 I0 J0
N3 G9 G3 W2 I0.875 K-0.125 <- R of the cut = 0.25
N4 L44 N2 N3
 
Last edited:








 
Back
Top