Machsupport Forum

Mach Discussion => General Mach Discussion => Topic started by: Mountainman on March 30, 2013, 09:41:19 PM

Title: Arcs and cutter comp
Post by: Mountainman on March 30, 2013, 09:41:19 PM
OK, My 1st program. 

In regards to making arcs, is I and J incremental or absolute in Mach3?  What if I am in G90 mode? 

I plan on cutting a path by programming the points of the outline and using both G41 and G42.  You see, I have a .375" cutter and I am going to for the first pass, G41 and use a P variable of .375 ( .750" diameter cutter), get to the end of the pass and then switch to G42 w/ a P of .3125, go back up that path but in reverse.  I want to go back and forth getting closer each time to the final dimension until I use a final P of .1854 as this whole operation has been a roughing cut in 4140 PH.  I will not be making any tool changes so I won't be using D variables.  From what I understand, I don't need any lead in moves when hitting the end of the path and changing between G41 and G42.  My question is this, will I need to include lead in moves because I am changing my P values?

       

Title: Re: Arcs and cutter comp
Post by: BR549 on March 30, 2013, 09:52:20 PM
Arcs, IJ mode? you can have it either way it is covered in the manual

Not a great idea to "try "and use the toolcomp offset to do your machining that way. Just program the moves as you need them. Go down the line move over a step over amount and go back to the beginning, Repeat until you are at the final value.

Just a thought(;-) TP

Title: Re: Arcs and cutter comp
Post by: Mountainman on March 30, 2013, 10:33:22 PM


Not a great idea to "try "and use the toolcomp offset to do your machining that way.
Just a thought(;-) TP


Please elaborate?  I used to make mock programs by drawing paths around my parts in CAD, that grew tedious and tiresome, especially if there is a function that can take care of that for me.  I also used to program using tool center paths and a buddy of mine that actually has experience doing this told me, learn cutter comp.  is cutter comp in mach not reliable? 

Title: Re: Arcs and cutter comp
Post by: BR549 on March 30, 2013, 11:12:52 PM
To use Cutter Comp you still program as tool centerline and you use the Comp to offset the toolpath by the value of the tool radius. BUT you have to use a leadin/out to bring the tool into play or out of play for the moves.

Best get a GOOD gcode manual to study as describing it in full here could take HOURS of typing(;-) Also note that MACH3 may have nuaisences that other favors of Gcode do not. So the basic's apply but the fine tuning may be MACH3 specicfic. Should be covered in the manual(;-).

(;-) TP
Title: Re: Arcs and cutter comp
Post by: Eradicatore on March 31, 2013, 01:07:38 AM
OK, My 1st program. 

In regards to making arcs, is I and J incremental or absolute in Mach3?  What if I am in G90 mode? 

I plan on cutting a path by programming the points of the outline and using both G41 and G42.  You see, I have a .375" cutter and I am going to for the first pass, G41 and use a P variable of .375 ( .750" diameter cutter), get to the end of the pass and then switch to G42 w/ a P of .3125, go back up that path but in reverse.  I want to go back and forth getting closer each time to the final dimension until I use a final P of .1854 as this whole operation has been a roughing cut in 4140 PH.  I will not be making any tool changes so I won't be using D variables.  From what I understand, I don't need any lead in moves when hitting the end of the path and changing between G41 and G42.  My question is this, will I need to include lead in moves because I am changing my P values?

Hi Mountainman,
   Too funny, I just noticed your post right after I posted a very similar question and have been beating my head trying to understand G02 and G42 for a few hours.  I think we may have similar questions, but also you seem to have a question that I have just learned the answer to I think.

   Go to the "Config" pull down menu and select "General Config...".  There in the middle you'll see "IJ mode" and you can select relative or absolute.

   For some reason this is "absolute" by default I think.  And it would seem that doing G02's with relative IJ's is way easier to code by hand.

   Anyway, I got that working fine, but see my other questions here:

http://www.machsupport.com/forum/index.php/topic,24178.0.html
Title: Re: Arcs and cutter comp
Post by: Mountainman on March 31, 2013, 10:02:24 AM

Hi Mountainman,

   Go to the "Config" pull down menu and select "General Config...".  There in the middle you'll see "IJ mode" and you can select relative or absolute.

   For some reason this is "absolute" by default I think.  And it would seem that doing G02's with relative IJ's is way easier to code by hand.

   Anyway, I got that working fine, but see my other questions here:

http://www.machsupport.com/forum/index.php/topic,24178.0.html


I use CAD in order to figure out the points of my cutter path.  I just set my datum on the workpiece where I want it and then I just transpose my points to the G code, so for me, absolute mode seems easier, no need to subtract anything.  So bottom line, we have the arc question answered, it does not matter if I am in G90 or G91.  What determines if I am using absolute or incremental IJ is in the general config menu.
Title: Re: Arcs and cutter comp
Post by: BR549 on March 31, 2013, 10:45:40 AM
actually you need to read the manual(;-)

G90 set abs motion
G91 set inc motion

G90.1 set abs IJ arcs
G91.1 set inc IJ arcs

The Gen config setts are just the defaults that Mach3 starts up with.

Just a thought, (;-) TP
Title: Re: Arcs and cutter comp
Post by: Mountainman on March 31, 2013, 02:05:45 PM
actually you need to read the manual(;-)

G90 set abs motion
G91 set inc motion

G90.1 set abs IJ arcs
G91.1 set inc IJ arcs

The Gen config setts are just the defaults that Mach3 starts up with.

Just a thought, (;-) TP

I'll remember to add G90.1 at the header of my programs so I don't have to worry about config settings.  Thanks, but what I really need help on is if knowing whether a lead in move is necessary when changing the P value in cutter comp? 
Title: Re: Arcs and cutter comp
Post by: Mountainman on March 31, 2013, 05:30:43 PM
It works ok, I see that lead in moves are not perpendicular to programmed path, so I see why lead in/out moves are used as to not disturb the material that should not be cut.  For my intenst and purpose it looks fine.  I tested it all out by fixturing some paper and chucking in a pencil. 

I also learned that my G code, the values that should have been - were all + and vise versa.  Then when I fixed it all up, the part was shown on teh screen as a mirror image.  My X axis seems to be in the wrong direction, how do I flip that? 
Title: Re: Arcs and cutter comp
Post by: BR549 on March 31, 2013, 06:00:54 PM
IF the Mach3 too lpath is showing the mirrored image then your Gcode is mirrored. IF the display is correct and it cuts mirrored then the motor is backwards.

The lead in / out  is ONLY there to give MACH3 room to do the tool radius comp move. IT is up to YOU to make sure the profile is fully cut(;-) as part of your programming in Gcode.

Just a thought, (;-) TP
Title: Re: Arcs and cutter comp
Post by: Mountainman on April 02, 2013, 08:52:37 PM
when I said that my X axis seems to be in the worng direction, I am talking about the image area, not the axis motor.  Teh tabels moves in teh driection of teh arrows on teh control pendant, so they are going in the right direction. 
Title: Re: Arcs and cutter comp
Post by: BR549 on April 02, 2013, 09:35:39 PM
OK IF the toolpath on the screen is backwards (mirrored ) then you are programming it backwards.

What type of machine is this Knee mill, Gantry mill, router. Does the spindle move in xy or does the table move XY?

Depending on the type machine as to which way it should move when you use the jog button. Direction is based on which way the perceived tool motion is.

(;-) TP

Title: Re: Arcs and cutter comp
Post by: HimyKabibble on April 02, 2013, 10:12:39 PM
Teh tabels moves in teh driection of teh arrows on teh control pendant, so they are going in the right direction. 

That is actually incorrect.  In the world of CNC, all motion is defined in terms of direction of movement of the tool, NOT the table.  Clicking on a "right arrow" control should move the TOOL to the RIGHT relative to the workpiece, or move the table to the LEFT on a milling machine.  So, your machine is setup backwards.

Regards,
Ray L.
Title: Re: Arcs and cutter comp
Post by: Mountainman on April 02, 2013, 10:23:00 PM
tool is stationary as this is a BP knee mill.  Let me think about that in my dreams tonight. 
Title: Re: Arcs and cutter comp
Post by: HimyKabibble on April 02, 2013, 10:55:18 PM
tool is stationary as this is a BP knee mill.  Let me think about that in my dreams tonight. 

Which means pressing the RIGHT arrow key should move the table to the LEFT.

Regards,
Ray L.
Title: Re: Arcs and cutter comp
Post by: BR549 on April 02, 2013, 11:03:58 PM
Ray is correct with a knee mill if you push X+ the table should go left which move the  tool tip right(perceived tool motion)

With Y push Y+ and the table moves towards  you (away from the column)

Mach3 will DISPLAY the code in the conventional MODE.   

(;-) TP
Title: Re: Arcs and cutter comp
Post by: Mountainman on April 03, 2013, 02:47:19 PM
OK, so the direction that I had my program in cad was right and when I transposed those points into G code that was also right and it displayed correctly on the VRO, but my X and Y is going in teh wrong direction so that means after I get this part made I should switch things around including my homing config screen. 
Title: Re: Arcs and cutter comp
Post by: garyhlucas on April 12, 2013, 07:42:44 PM
Mountainman,
If your machine has only a little backlash and can handle climb milling, then I would climb mill the part the whole time.  Conventional milling has the cutting edge sliding over the surface until the material is thick enough to peel a chip.  This wears the cutter much faster.  Climb milling starts with a full chip and the chip thins until it breaks off, which is much better. In most cases the finish is better too.

When programming manually from a CAD drawing I always program right on size and use cutter comp.  I always put the tool path in a subroutine and just set cutter comp, call the sub, adjust comp, call the sub.  I program the subs in incremental.  That way I can always position it anywhere, or even use it in multiple locations.  I also like to use undersize cutters on pockets to sweep the corners with the cut, not crash to a stop and change direction. This got me on good terms with the guy in the tool room because I actually asked for resharpened end mills, and he always made sure I got freshly sharpened ones.  He did a good job too, they always seemed to cut better than new ones.

One of the machinists said I was wasting time with rapid moves back to the start of the tool path and should program it the way you want to.  I pointed out to him that if we had lots of parts to do that would be a good idea.  With batches of ten or less you really can't justify the extra coding and testing to be sure it works.

Gary H. Lucas