What's new
What's new

Trachoidal milling programming by hand

Traegerdacoda12

Plastic
Joined
Sep 25, 2019
I'm wondering if it's possible or atleast realistic to HAND WRITE trachoidal milling tool paths. I can't really find anything about it online except for using cam software. If you know how to do it can u post an example? Thank you
 
You could try to draw out circles on graph paper or in CAD with whatever parameters you like but it would be really time consuming. An example would just look like a series of increasing circles based on stepover then trimmed to fit to stock with fillets to return to next position ad nauseum.
 
Theoretically possible, but why would you? Even the free CAM software does it these days. You can make turbines on a manual Bridgeport too, but why?

I had my head up my rear when I got my first CNC and didn't think to look for free software. I hand programmed a program not being aware that new free software was out there that could do it. I programmed overnight by hand and what took me 15 hours took 15 minutes by free software. I programmed by hand exactly once. And lets face it, we all know it was not as clean as a computer generated path. Nothing I was proud of except to have the courage to admit it in public.
 
Of course you can do it.

Simplest example:

g91 G3 j3
g1 x1
repeat.


I'm actually in the process of completing a full trochoidal macro right now.
 
No, if you knew the math behind the thing you can not spell you would not try.
Don't mean to be a ass but it involves lots of lines of code.
Slots, not so hard, pockets complicated.
Bob
 
Trochoidal path on a slot isn’t difficult. Make a sub program of one loop and a step-over in incremental, then call it, followed by an L# for the number of times you need it to repeat to cut the slot.
 
No, we don't aall know that. Hand-written programs are frequently - perhaps even usually - better than computer-generated programs.

They just take a lot longer to create.

How's that even possible, please explain?

Surfcam does exactly what I want it to do. It's never even occured to me to hand write a program ever, no need to.

There's been the odd occasion where I might have edited a program to change a plunge point possibly that Surfcam created, but that's rare.
 
FWIW, I plan on writing one for slots on my mill also.

I planned on asking for a code example too. I thought it was just a series of G3's, at least that's my plan on how to write it. I would like to confirm this Once done, just call it up and change tool, start location, end location, width, depth, step over, etc.

Guess I'm old school. nearly all my work is extremely simple gcodes and gcode macros, just LOTS of loops. Plus I design as I go for the assemblies under construction. Sketch what I need, start cutting. write next segment while machine is running.


PS. I would like to know if this method cuts air 1/2 the time with complete G3s. or 180-G3, advance,180-G2, advance. This seems more efficient to me.
 
I had talked to a company and this is what they wanted me to program everything that came in the door. Then said by hand no CAD what so ever pay was like 12-15 bucks top dollar pay he said. I told him where to stick it and 3 years their ad still keeps popping up.
 
How's that even possible, please explain?

Surfcam does exactly what I want it to do. It's never even occured to me to hand write a program ever, no need to.

There's been the odd occasion where I might have edited a program to change a plunge point possibly that Surfcam created, but that's rare.


Well, for example, broaching a hex by picking one corner out at a time, stepping out in X, doing each corner once at each X depth, with a total of 10 steps in X... CAM Code would be hundreds of lines long.... Or it can be hand written with two nested DO/WHILE loops that total about 15 lines of code.
 
Of course you can do it.

Simplest example:

g91 G3 j3
g1 x1
repeat.


I'm actually in the process of completing a full trochoidal macro right now.

Right... now write a Trochoidal macro to mill anything other than a straight line.
 
FWIW, I plan on writing one for slots on my mill also.

I planned on asking for a code example too. I thought it was just a series of G3's, at least that's my plan on how to write it. I would like to confirm this Once done, just call it up and change tool, start location, end location, width, depth, step over, etc.

Guess I'm old school. nearly all my work is extremely simple gcodes and gcode macros, just LOTS of loops. Plus I design as I go for the assemblies under construction. Sketch what I need, start cutting. write next segment while machine is running.


PS. I would like to know if this method cuts air 1/2 the time with complete G3s. or 180-G3, advance,180-G2, advance. This seems more efficient to me.


Karl,
It does essentially cut air. I believe the premise of using all G3 is that the machine stays in a constant circular motion rather than the start/stop of switching directions going from G2 to G3. The changes in accel/decel would outweigh the benefits and it's probably quicker to just keep swinging the same direction.
 
Well, for example, broaching a hex by picking one corner out at a time, stepping out in X, doing each corner once at each X depth, with a total of 10 steps in X... CAM Code would be hundreds of lines long.... Or it can be hand written with two nested DO/WHILE loops that total about 15 lines of code.

True enough, but unless you are limited in memory, or have a very slow pc, it doesn't much matter.

Also an advantage of cam (maybe not all, don't know) , is there is a place to specify a back feedrate and 'micro' lift distance so you are not draggin the tool back across an already cut area at your feedrate, instead lift the tool .01" (my default) and feed back to the next cutting move at 300+ ipm.
 
How's that even possible, please explain?

Surfcam does exactly what I want it to do. It's never even occured to me to hand write a program ever, no need to.

There's been the odd occasion where I might have edited a program to change a plunge point possibly that Surfcam created, but that's rare.

Some other examples:

Post a CAM program for threadmilling with a single point tool, or helixing a bore. Unless you have spent a lot of time or money on your post, it's going to spit out a whole lot of lines that can be done with 1 line in G91 with an L.

I also see a lot of wasted lines for lead in/out and approach / retract movements. 3 Z- moves in a row when it could have been 1, etc.

Many CAM programs I see are 5-10 times more memory used than the hand-written version of same toolpaths. As long as memory isn't an issue, it doesn't really matter though, apart from being harder to follow.
 
Right... now write a Trochoidal macro to mill anything other than a straight line.
Hum, okay.

Code:
:9015(TEST)
G90G54X0Y0Z50S5000M3F1000
M98P9016L1

:9016(M-CIRCTROCG3) 
(MILLS A CIRCULAR 90 DEGREE SLOT WITH RADIUS 50 AND INNER RADIUS 30.)
(TOOL DIAMETER IS 10.)
(FLATTENED RETRACTION /8)
(COULD BE MADE A PRODUCTION MACRO.)
G0 X45Y0
G0 Z5
G1 Z0
#105=0(ANGLE COUNTER)
WHILE[#105LT90]DO1
G3X[COS[#105]*35]Y[SIN[#105]*35]R5
G3X[COS[#105]*45]Y[SIN[#105]*45]R40
#105=#105+2
G3X[COS[#105]*45]Y[SIN[#105]*45]R45
END1
G0Z50
M99

tg3.jpg

Happy? By the way thanks for getting me motivated to sketch the trochoidal g2-g3, I'm really not done with the g1 one, it requires different optional toolpaths and vertical skews. (Also varying feeds.) (Would G8/G05 fix the feeds if I decide to radius compensate the sh*t? Feedback welcome.)
 
Last edited:
PS. I would like to know if this method cuts air 1/2 the time with complete G3s. or 180-G3, advance,180-G2, advance. This seems more efficient to me.
It may be slightly more time efficient but it puts a lot more stress on the tool, also switching conventional-climb all the time.

See the little snippet I posted, that should give you an idea. There are tons of strategies.

One is the simple circular trochoidal (full G3), that cuts a lot of air.

Then you have the one with the back-end flattened. Cuts less.

Then you have the one with G1 back-end. Cuts less than above.

For wide slots you also have the ones where you have a radius in, a g1, a radius out and retracting, a g1 and a g3 back to the starting position and advance.

Oh and finally you have the circular advance plus the elliptic retract, that's what I'm coding right now. I'm no master of physics but it's said to be best for tool life.

Point being the more abrupt tool path change the more stress on the tool, the more G-forces, the more chance something comes unstuck.

Abrupt path changes on high-feeders wreck everything. Most people who use trochoids use them on smaller solid end mills, that's obviously safer.

Dunno if that helped.

(PS obviously you increase feed on the backburner. Didn't bother including it in the smallish code I wrote above.)
 
I hear ya on the abrupt direction changes. stick with full G3s. simpler and better.

i am a baseball fan. While watching the twingkies hit homer #300 I wrote a trichordal macro to make a slot in any 360 degree direction. i'll test it tomorrow.
 
Well, for example, broaching a hex by picking one corner out at a time, stepping out in X, doing each corner once at each X depth, with a total of 10 steps in X... CAM Code would be hundreds of lines long.... Or it can be hand written with two nested DO/WHILE loops that total about 15 lines of code.

And the great part about loops is if it's wrong, you only have to change it in one place.
 








 
Back
Top