Trying to get G03's instead of lots of short G01 moves

[hooverwelding]

 So I have this attached part, 10" dia. coned to 2".

 I would like to rough it out with 1.4" step downs on the mill so it works better on my smallish lathe to finish to the cone shape.

 I can get it to look like I want with 3D adaptive and setting the step downs, etc. but when I post the code it is about 34,000 lines and mostly short G01 moves (and my 7000M Okuma control doesn't hold near that much code).

 I tried putting the tolerance and smoothing higher (.005-.010) but it didn't seem to help much.

 Am I missing something here?

  Thanks in advance!

[LibertyMachine]

I think the solution is going to be found in the post processor. I'll start digging into it, but just wanted to get the ball rolling in your favor.

Running it through the new Haas post that comes with Fusion, I get 417 lines of code

Running it through an Okuma or Fanuc post gives me 15,480 lines. Both of these are the "built-in" posts

*EDIT* I "think" it's because of the allowSpiralMoves in the Haas post. I'm out of time for tonight, but if someone is inclined to pick that ball and run with it 🙂

[LibertyMachine · Accepted solution]

Well, I had a few minutes more to play with this and I ported the spiral syntax over to the Okuma post. See attached.

Changes made:

1)

allowSpiralMoves = true;

2) 

var maximumCircularRadiiDifference = toPreciseUnit(0.005, MM);

3)

function onCircular(clockwise, cx, cy, cz, x, y, z, feed) {
  if (isSpiral()) {
    var startRadius = getCircularStartRadius();
    var endRadius = getCircularRadius();
    var dr = Math.abs(endRadius - startRadius);
    if (dr > maximumCircularRadiiDifference) { // maximum limit
      linearize(tolerance); // or alternatively use other G-codes for spiral motion
      return;
    }
  }

All these lines I ripped out of the Haas post and stuck em in the Okuma. You are now able to post out at 479 lines of code 🙂

Do be warned: I've got no idea what this would do to anything else in the program. Proceed with caution!

What the heck?! Can't attach a .cps file? See the .zip file

[hooverwelding]

Wow Seth!     Good, Fast, Cheap, and I got all three 🙂

 I used the post processor you attached and tried the code on the machine (after a couple edits to match the format I had in the post I was using) and it worked great, in dry run at least.

 I attached a zip file containing the post processor I was using that I got from Scott Moyse on here a couple years ago.

 As I can't quite trust myself changing things in the post processor, would you want to edit the post you had sent me sometime? Here is what I would like:

1. "$" before file name in first line and ".MIN%" after file name

2. On about line N3 instead of sending Z to 400, post "G30 P1" (tool change position)

3. Again at end, instead of Z400 X-400 Y 400,  post "G30 P1"

4. At end of file, last line, post "%"

And I've often wondered, why turn off the spindle first, and then the coolant, at a tool change or end of program? Seems to me it would be better to turn coolant off first so some coolant spins off and the tool isn't dripping wet when put away. There is probably a reason for this that I didn't think of......

  Thanks so much!

Carl

Here is what one of the files looks like from what I was using.

$OENGRAVE.MIN%

N1 G40 G80 G90 G94 G17

N2 G20

N3 G30 P1

　

N5 M09

N6 T70 M06

N7 S3000 M03

N8 G15 H01

N9 M08

.....

N2190 G00 Z0.5

　

N2191 M05

N2192 M09

N2193 G30 P1

N2196 M02

%

[hooverwelding]

I noticed there is a newer Okuma post processor in post processor section at autodesk.com

  Carl

[hooverwelding]

 OK, thought I might post an update.

I downloaded the newest Okuma post from Autodesk and modified it using some of the things I wanted from my old post (from Scott Moyse) and the spiral stuff from the post from Liberty Machine, thanks again Seth, for your help on this.

I thought someone might share of their knowledge yet and explain why turn off the spindle first and then the coolant? (see earlier post)

  Thanks, Carl

[LibertyMachine]

Sorry for the delay in response, been a busy morning.

Personally, I see no reason to turn the spindle off first. My post (Fanuc) produces this:

G0Z.1M9

G0G49

G53Z0M19

M1

This turns off coolant, cancels tool length offset, and then turns the spindle off on it's way home

[Anonymous]

If your using HP CTS then it helps a bit to turn off the coolant first especially if using small tools to allow all the pressure to bleed off prior to a tool change, otherwise I can't think of a reason why it would make much difference.

[Anonymous]

Got to looking at our Okuma post and noticed it outputs G1 instead of G3's for circular interpolation as well, tested code of a 6" OD @ .200" step over and it generated all most 2,900 lines of code!

Not real proficient at editing a post in Java so some guidance here would be welcomed, File attached.