Author Topic: Hidden feature in profile MOP ?  (Read 3124 times)

Offline dh42

  • Administrator
  • CNC Jedi
  • *****
  • Posts: 6209
    • View Profile
    • Cambam V1.0 French Doc
Hidden feature in profile MOP ?
« on: May 03, 2018, 23:47:48 pm »
Hello,

Today, while trying to find a problem on a friend's file, I discovered something I don't know with profile mops.

You already know that profile mop don't worry about the Z position or flatness of a polyline and don't follow the Z variations of this one.

It's not totally true ; if a profile mop use a roughing clearance = - 1/2 tool diameter (so it follow the polyline without radius comp.), then it works as a engrave mop and the toolpath follow the Z variation too ! ; in addition lead-ins are also usable (no leadin in an engrave mop).

++
David
« Last Edit: May 03, 2018, 23:49:22 pm by dh42 »

Offline lloydsp

  • CNC Jedi
  • *****
  • Posts: 8360
    • View Profile
Re: Hidden feature in profile MOP ?
« Reply #1 on: May 04, 2018, 00:39:03 am »
Huh?  Really?  I can do profiles with varying Z on the line?  REALLY?  AND with lead-ins?  OH!

OH, MY!  I must experiment with that!!!

Thank you David!

LLoyd
"Pyro for Fun and Profit for More Than Fifty Years"

Offline dh42

  • Administrator
  • CNC Jedi
  • *****
  • Posts: 6209
    • View Profile
    • Cambam V1.0 French Doc
Re: Hidden feature in profile MOP ?
« Reply #2 on: May 04, 2018, 00:52:01 am »
Yep, but only if you use a negative roughing clearance = tool radius ; if not, the profile act as usual and produce "flat" toolpath.

note also that the way the stock surface Z coordinate is used is not the same than as an engrave mop .. but it's not totally clear for me at the moment ... it seems to be relative to the fist point of the polyline ...

++
David
« Last Edit: May 04, 2018, 00:56:16 am by dh42 »

Offline dh42

  • Administrator
  • CNC Jedi
  • *****
  • Posts: 6209
    • View Profile
    • Cambam V1.0 French Doc
Re: Hidden feature in profile MOP ?
« Reply #3 on: May 04, 2018, 01:32:56 am »
more experiments ..

unfortunately it don't works with side profile ...

concerning the way the stock surface is used:

with an engrave mop, the Z position of each point of the polyline is added to the SS value in the MOP, so for a line that go from Z = 50 to Z = 40 and with SS = 0 in the mop, toolpath will go from 50 to 40.

with a profile mop, with the same settings and if the start point of the cut is the one at Z=50 ; this point is used as reference for the SS, and is aligned on Z= 0, so the toolpath will go from 0 to -10 and if it is the point at 40 that is the first point of the cut, the toolpath will go from +10 to 0. It is the start point of the cut that is used as reference, not the first point of the polyline, so changing the machining direction (climb, conventional) and/or the start point of the polyline change also the Z position used as reference for SS ... be careful !! and play with this 2 settings to get the proper "altitude" for the toolpath ... and internal/external settings change also this behavior ;)

++
David
« Last Edit: May 04, 2018, 01:38:08 am by dh42 »

Offline dh42

  • Administrator
  • CNC Jedi
  • *****
  • Posts: 6209
    • View Profile
    • Cambam V1.0 French Doc
Re: Hidden feature in profile MOP ?
« Reply #4 on: May 04, 2018, 03:05:25 am »
.... and another test with a closed polyline (an inclined rectangle) cut with a progressive ramp (spirale)

the GCode is also modified to do a tool compensation with G41 so we get the same as a profile with no roughing clearance

View in Mach3

.

Blue lines = the toolpath with no radius compensation done by CB
White lines = the compensated toolpath calculated by Mach3 with G41

The change in the Gcode produced by CB to use the tool compensation are only

G0 X-10.0 Y-10.0
G1 G41 X0.0 Y0.0

in place of
G0 X0.0 Y0.0

++
David
« Last Edit: May 04, 2018, 03:11:22 am by dh42 »

Offline Garyhlucas

  • CNC Jedi
  • *****
  • Posts: 1380
    • View Profile
Re: Hidden feature in profile MOP ?
« Reply #5 on: May 04, 2018, 13:26:00 pm »
Just a little warning. I programmed almost exclusively using g41, g42 before using cambam. One practice that kept me out of trouble is Never apply the offset to a cutting move, Always apply the offset while above the part. Do this with a dummy move, I always used a 0.010” move in the cutting direction. When the offset gets applied you see the tool move to the side by the radius and if it went the wrong way you have time to hit the wed button.
Gary H. Lucas

Have you read my blog?
 http://a-little-business.blogspot.com/

Offline kvom

  • CNC Jedi
  • *****
  • Posts: 1587
    • View Profile
Re: Hidden feature in profile MOP ?
« Reply #6 on: May 04, 2018, 23:48:09 pm »
I may be dense but I don't see the advantage of this "undocumented feature" (another name for a bug?).  This kind of thing is also likely to disappear in a future release if it's unintentional.

Offline StefanR.

  • Ewok
  • *
  • Posts: 25
    • View Profile
Re: Hidden feature in profile MOP ?
« Reply #7 on: May 07, 2018, 12:16:46 pm »
Turns out that a tool radius of 0 does the same, but reversion of polyline and outside/inside mixes up the Z-coordinates..  Wich is the same behaviour for Roughing clearance of -1/2 diameter. So: might come in handy if properly checked and verified..

Offline StefanR.

  • Ewok
  • *
  • Posts: 25
    • View Profile
Re: Hidden feature in profile MOP ?
« Reply #8 on: May 09, 2018, 06:58:04 am »
To correct the z-coordinates, it appears that you can modify the difference in z-value using the target depth...

Offline pixelmaker

  • CNC Jedi
  • *****
  • Posts: 1788
    • View Profile
    • pixelmaker
Re: Hidden feature in profile MOP ?
« Reply #9 on: May 09, 2018, 08:31:11 am »
David,
I remember once Andy wanted to do all the 2.5D work in one mop. There should be no difference between profile and engraving. That's where these properties come from. I've known her and I've used her for ages. It's been a long time (2009-2010 Version H, peut-être), and you just forgot.
In the engraving mop, the toolpath is calculated in relation to the drawn line. If depth increments are used, they start in relation of the line.
With the profile mop, the toolpath is created in relation to Z=0 and the depth increments are also calculated from there. The distance between the toolpath and Z=0 is calculated from the starting point of the toolpath. If a target depth of -10 is set for workpiece surface = 0, the toolpath starts at -10
Andy then gave up the project again because he would have had to rewrite too much. Therefore we got Corner Overcut and some other different functions between profil and engrave.


ralf
« Last Edit: May 09, 2018, 08:38:37 am by pixelmaker »