how do you post to use G19 (YZ plane for circular interpolation)

[powerfulp]

Hello,

 

I have to do some G19, YZ circular interpolation, on a horizontal boring mill. So, the end point of the arc is defined by the Y word and Z word, and the distance from the start of the arc to the center point of the arc parallel to the Y-axis is defined by the J word, Z-axis by the K word.

 

I am using Mastercam X6, the latest and greatest version, mill-1. We usually only program 3-axis linear work (X,Y,Z) using G17 for circular interpolation, with the B-axis only for positioning. I have no problem programming this way in mastercam. Anyway, if I was standing and look straight ahead at the part, starting at the top, the geometry I'm trying to mill arcs 100mm radius towards you (Z+) and down (Y-), then is supposed to mill at a 20 degree angle for a bit (Z+Y-), then arc a 100mm radius the opposite way, using Z+Y- again, until it is flat and just moving straight down in the Y-axis. I hope I've explained that good enough.

 

So, I draw up this funky little radii feature and program a cutter on it. First of all, when I watch it in back plot, the mill does not follow the line like I want it to. Remember, it's milling from the front with the Z-axis moving out and the Y moving down. So the center of the cutter is on the line which means my "depth", or Y-axis, is down too low because I really want the front of the cutter to be following this line. That's the first problem. Secondly, when I post, I get all kinds of errors. Stuff like this:

 

 

UPDATEPOST Version 14. was used to modify this file.

01 Feb 2013 03:36:18 AM - <2> - The file was modified by this product on 22 Jan 09 12:52:44

01 Feb 2013 03:36:18 AM - <2> - The post was written to run with Mastercam Version 14.

01 Feb 2013 03:36:18 AM - <2> - The post product type is Mill.

01 Feb 2013 03:36:18 AM - <2> - Initialization of pre-defined post variables, strings, postblocks was successful.

01 Feb 2013 03:36:18 AM - <2> - Search for defined post variables, strings, postblocks was successful.

01 Feb 2013 03:36:18 AM - <2> - CONTROL DEFINITION - Post variable 'ltol$' was re-initialized from 0.0005 to 0.002

01 Feb 2013 03:36:18 AM - <2> - CONTROL DEFINITION - Post variable 'atol$' was re-initialized from 0.5 to 0.01

01 Feb 2013 03:36:18 AM - <2> - CONTROL DEFINITION - Post variable 'err_file$' was re-initialized from 0. to 1.

 

And so on...

 

I can choose to look at the code it created and instead of giving me arcs with J's and K's, I get points. A bunch of small increment Y-axis and Z-axis moves. I do not want this, either.

 

Do I need an option (or a higher version than mill-1) to mill this path and have it post correctly? Or is there some way to get this to post using G19? (And also, how do I get the front of the cutter to follow the line I created?).

 

I know this is a long one, hopefully someone has read it till the end and can help.

 

Thank you.

[Colin Gilchrist]

Hi powerfulp,

 

This should be fairly easy to fix.

 

First, in your toolpath, turn on the toolpath filter. There are checkboxes that you can set to "create arcs in YZ" and "XZ". This will give you the G19 arcs you are looking for.

 

The issue with the tool not following the geometry is a little harder with Mill Level 1. Right now the tip of your tool is following the geometry, which means at the top of the arc, the tool will be tangent, but as it starts following the arc "down", the tip will gouge below the arc.

 

A surface type toolpath will take this into account, and maintain tangency of the tool, (which offsets the tip).

 

Mill Level 1 does have some limited surfacing ability with the "wireframe" toolpaths. These toolpaths can be used to get the motion you want, and have some ability to offset the tool tip, to maintain tangency with the geometry.

[powerfulp]

Thank you, I found it and it worked! Cool.

[powerfulp]

I need to re-visit this....

 

I did what Colin instructed me to do and with the geometry I had at that time, it worked by just turning on the toolpath filter.

 

However, that was just practice, and I was doing it with a straight line, going up and down. In reality, I need to rotate the toolpath 22.5 degrees, then do the same thing (so it will be arcing in Y & Z and moving over in X simultaneously). I figured this would be something like helical interpolating, using X & Y to arc and Z moving linearly, and it would post using G19 with J's and K's for the Y's and Z's, with X moving accordingly. That is not what happened when I posted. We are back to it plotting a bunch of points for each axis, which is not what I want.

 

Anyway to get it to do what I'm looking for?

 

Thanks for any help.

[Colin Gilchrist]

Can you upload a file so someone can take a look?

[powerfulp]

Ok, I've only looked for a minute but how do you go about uploading a file here?

[powerfulp]

This is what is posted ... (I put notes in the program explaining what I want to happen vs what's really happening) :

 

O6986

N100 G20

N102 G0 G17 G40 G49 G80 G90

( 2.5" END MILL - MOVED X9.3000 )

N104 T317 M6

(NOTE: THIS PASS IS NOT MOVING IN X-AXIS SIMULTANEOUSLY )

( WHILE ARCING IN Y & Z AND POSTS HOW I WANT IT TO POST)

( WITH G2'S AND G3'S )

N106 G0 G90 G54 X8.5921 Y14.5478 S1528 M3

N108 G43 H317 Z.25

N110 Z.2

N112 G1 Z0. F24.45

N114 Y7.496

N116 G19 G2 Y6.1495 Z.2374 J0. K3.937

N118 G1 Y5.0204 Z.6484

N120 G3 Y3.6738 Z.8858 J-1.3466 K-3.6996

N122 G1 Y-1.6834

N124 Z1.0858

N126 G0 Z1.1358

N128 X4.3868 Y13.7113

N130 G17

N132 Z.25

N134 Z.2

N136 G1 Z0.

( NOTE: THIS PASS IS MOVING IN X-AXIS SIMULTANEOUSLY )

( TO ARCING IN Y & Z )

( I WANT THIS PORTION OF THE PROGRAM TO USE G2'S AND G3'S )

( LIKE THE ARCING DONE ABOVE ... BUT WHEN MOVING )

( IN THE X-AXIS ALONG WITH ARCING IN Y & Z - THESE POINTS )

( ARE POSTED INSTEAD )

N138 X7.0854 Y7.1963

N140 X7.1605 Y7.015 Z.0049

N142 X7.2354 Y6.8342 Z.0196

N144 X7.31 Y6.6542 Z.044

N146 X7.384 Y6.4756 Z.0781

N148 X7.4572 Y6.2988 Z.1217

N150 X7.5295 Y6.1242 Z.1749

N152 X7.6007 Y5.9523 Z.2374

N154 X8.0328 Y4.9091 Z.6484

N156 X8.104 Y4.7372 Z.7109

N158 X8.1764 Y4.5626 Z.7641

N160 X8.2496 Y4.3858 Z.8078

N162 X8.3236 Y4.2072 Z.8419

N164 X8.3981 Y4.0272 Z.8663

N166 X8.473 Y3.8464 Z.8809

N168 X8.5481 Y3.6651 Z.8858

N170 X10.5982 Y-1.2843

N172 G0 Z1.1358

N174 M5

N176 G91 G28 Z0.

N178 G28 X0. Y0.

N180 M30

 

Some other info:

 

1.) The machine definition I'm using is MILL DEFAULT (I hope that's what you're looking for).

2.) The machine control settings for arcs are: Supports arcs in XY plane, XZ plane & YZ plane. Arc center type is set to Delta start to center. Arc break options: Don't break arcs. I am only allowing 360 degree arcs in XY plane. Don't know what else you'd like to know.

3.) I've attached the actual file I'm working with.

4.) Mill contour is the type of toolpath I selected.

 

Thanks!

YZ ARC WITH X-AXIS MOVING.zip

[powerfulp]

nobody interested in this one anymore? or do you need more info? Or ??

 

thanks for any help

[Allan]

Your Red arc is parallel to the Y axis that is why you are able to filter for an arc in YZ.

The Blue arc is not parallel to any axis and will never produce an arc with Mastercams arc filter.

This type of arc could be cut but only on a control that would allow you to define the arc plane like a Siemens 840, then you would also require a 3rd party filter like Metacut.

 

BTW:

Your cut parameters are a little strange as well, stock to leave is set to minus half of the tool; why not just turn cutter compensation off?

 

 

Allan

[powerfulp]

So you're saying Mastercam will never post an arc using G19 in Y & Z if moving in the X-axis simultaneously? I would have never thunk it. I figured it would be something like helical interpolation. Well, since I couldn't get Mastercam to post it, I programmed it manually and this is some of the code that worked (cut geometry correctly/no arc error alarms):

 

 

N15960 G0G90G54X-11.6440Y6.4000S495M3

N15970 W-2.0000

N15980 G43Z2.0060H129

N15990 G19

N16000 G1X-11.6440Y2.8365F30.0

N16010 G2X-11.0862Y1.4899Z2.2434J0.0000K3.9370F15.0

N16020 G1X-10.6180Y.3608Z2.6544

N16030 G3X-10.0602Y-.9858Z2.8918J-1.3466K-3.6996

N16040 G1X-9.8000Y-1.4000Z2.9000

N16050 G0Z5.0000

 

 

And yeah, I'm sure I have some things setup goofy, I don't have much experience with Mastercam. We've had it for over a year but I've probably worked on it a total of a week or two. I'm planning on working on it much more in the near future....

 

Anyway, thanks for the info.

[Allan]

I programmed it manually and this is some of the code that worked (cut geometry correctly/no arc error alarms):

 

"Correctly" would be open to interpertation, your code looks like this in a backplot:

Hardly matches your geometry in Mastercam, looks like 4 line segments.

 

There is a chook called arc3d it will attempt to filter for helixes, but with the file you have there is no way a helix will fit to an arc drawn in the side view rotated 22.5 degrees in the top view, no way ever.