Newbie- g83 problem

[basswakr]

i have a multicam router
having problems with g83
material top 1
surface is 0 (bot. of mat.)
safe rapid 1.5
peck dis. .5
total peck depth .875

problem is it drills to .125 1st
then raises & pecks back down to .125
i want it to peck on the way down
can anyone tell me what to change to make it happen?

ex:

G75
G97 S2000
G00 T14
G00 X2.2201 Y4.1962
M12
G83 R-1.25 Z-0.125 D-0.5 F0.833
M22
G00 X5.1576 Y4.1962
M12
G83 R-1.25 Z-0.125 D-0.5 F0.833
M22
G00 X8.2826 Y4.1962
M12
G83 R-1.25 Z-0.125 D-0.5 F0.833
M22


thx
mike

[dertsap]

your r value is deeper than your z value , your drilling in reverse , lucky your cutting wood , steel wouldn't be so forgiving

[basswakr]

no i think that part is right
it clears the part just fine
remember i am working from the bottom up


thx
mike

[Superman]

Originally Posted by basswakr i have a multicam router having problems with g83 material top 1 surface is 0 (bot. of mat.) safe rapid 1.5 peck dis. .5 total peck depth .875 problem is it drills to .125 1st then raises & pecks back down to .125 i want it to peck on the way down can anyone tell me what to change to make it happen? ex: G75 G97 S2000 G00 T14 G00 X2.2201 Y4.1962 M12 G83 R-1.25 Z-0.125 D-0.5 F0.833 M22 G00 X5.1576 Y4.1962 M12 G83 R-1.25 Z-0.125 D-0.5 F0.833 M22 G00 X8.2826 Y4.1962 M12 G83 R-1.25 Z-0.125 D-0.5 F0.833 M22

Your values in the g-code are incorrect
G73 = peck cycle ( keep pecking until Z value is reached )
G83 = deep hole peck cycle ( full withdrawal after each peck )
X Y = co-ordinate of hole
Z = final depth of hole
R = retract plane ( must be higher than Z )
D = peck depth ( -ive )
F = feedrate

your code should be
G83 R1.25 Z0. D-0.5 F0.833
you also can have
G83 X8.2826 Y4.1962 R1.25 Z0. D-0.5 F0.833
machine will rapid to XY
then rapid to R
peck drill from R to Z in D increments
rapid back to R
depending on machine settings it may go higher to it's initial level

[basswakr]

alright
i must have more wrong here with my post
i took the - off but now it just drills with no pecking.

any more ideas ?

thx
mike

[stevo1]

Originally Posted by basswakr problem is it drills to .125 1st then raises & pecks back down to .125. i want it to peck on the way down

What do you mean it drills to .125 + or -? With a G83 cycle it feeds your pick then returns to the R-plane after every pick. So if it is feeding to .125 which you have set as your Z I would suspect it does not like that. I have never set up a part this way. I would assume a lot of your problem is calling Z0 the bottom of the part then trying to manipulate your Z and R to accomodate to drill properly.

What is your initial Z move? Are you telling it to go Z(+#) above the part??

Stevo

[basswakr]

ok thx for all responses so far , getting a lot more help than i expected

found the problem i am missing the Z after my G00 X2.2201 Y4.1962

G75
G97 S2000
G00 T14
G00 X2.2201 Y4.1962 add this (((Z-1.5))) this makes it work right any ideas?
M12
G83 R-1.25 Z-0.125 D-0.5 F0.833
M22
G00 X5.1576 Y4.1962
M12
G83 R-1.25 Z-0.125 D-0.5 F0.833
M22
G00 X8.2826 Y4.1962
M12
G83 R-1.25 Z-0.125 D-0.5 F0.833
M22



any idea what to change in my post to make it add that?

thx
mike

[stevo1]

That's why I asked about your initial Z level. The initial Z point is the position of the drilling axis when the canned cycle cancellation state is switched to the canned cycle mode. This Z position is needed before you switch to canned cycle mode.

You can return to the initial point level with a G98 or the R point level with a G99.

Stevo

[basswakr]

stevo

u r correct

but where do u add that in the post?

[stevo1]

Originally Posted by stevo1 What is your initial Z move? Are you telling it to go Z(+#) above the part??

I apologize I did not really spell it out. But that is what I meant by your first Z position. I should have just stated you need a Z move before going to canned cycle. Sorry.

Stevo

[basswakr]

ok thx for all the help
got it fixed
post outputs correctly now.


M90
G90
G70
G75
G97 S1500
G00 T1
G00 Z-1.5
G00 X6. Y6.
M12
G83 R-1.25 Z-0.25 D0.25 F1.667
M22
G98 P147 D1
M02

[HAR]

Mike,

It was interesting reading your thread today as I was going through the same excercise but was unable to post as it took about 6 hours to get my registration through.

I am surprised your code is working as it is not working on my machine. I too have a Multicam machine and am wondering what is different from your machine to mine.

I have been programming for our Multicam machine for about 5 years now and just today decided to try to use the G83 canned cycle and cannot figure it out. I may be able to shed some light on Stevo's remarks...

Mike has mentioned that we are working form the bottom up...Multicam for whatever reason, works where negative values are above the table and positive values are below. This is backward from all other machine manufacturers I have seen. This situation makes it very difficult to get help from anyone but Multicam or other Multicam users and Multicam is not very good at support of G Codes, IMHO...

I am actaully re-writing some software I wrote a few years ago that generates the code for our machine and I am hoping to market it soon. I had written my own "Peck" routine using G01 and G00 commands and just decided to try the canned cycle. I figured why not use short hand if I can.

Here is my code using G83 to drill 1 hole...

(Date 12/16/2008)
(Path D:\Hal's Stuff\My Documents\Drawings\1100\)
(Name Point)
(Home = X110.000 Y13.000 Z-8.000)
(Clear Level = -1.250)
G90
G75
G00 T2 (1/4" Drill Bit)
G97 S5000
G00 X4.000 Y4.000 Z-1.250
(BeginContour 1)
M12
G83 R-1.125 Z-0.250 D0.250 F0.833
M22
(EndContour 1)
G00 Z-1.250
G00 X110.000 Y13.000 Z-8.000
G90
G97 S5000
M02

As you can see, my values are similar to yours. My material is 1" thick and I am trying to drill a 1/4" hole to within 1/4" of going through my board. I am asking that the peck cycle return to a level of 1.125" or .125" above my material between pecks. I am wanting the pecks to take out .25" of material each.

When I look at other controller (fanuc) code, all 3 of these values (R, Z and D) are positive so with Multicam saying negative numbers are above the table it is hard to distinguish what if any vales need to be positive for the cycle to work. Making all 3 values negative makes the machine continue to move "up" higher and higher after each cycle and does not end until it max's out.

If I might ask, could I get you to copy this code into a file and see if it works on your machine? If it does, I might need to see if there is a new post processor I need to make my machine understand this canned cycle.

My machine kind of pecks, but it moves down to the bottom level of .25" with each peck....wrong!

In addition to this, I need to figure out how the G83 cycle should work in the case we want to use "relative" or G91 mode in lieu of "absolute" code or G90.

Thanks for any help that might come my way,

Hal