HELP!!!!!!!!!

[buck30]

we just got a new robodrill in and the guy from methodas did a couple of things with my MC to make thimngs go smothly. However now my Centroid is doing funny things, below is a simple test program i put togeather

 

%

N10 ; PROGRAM NAME - TEST

N20 ; DATE - 19-04-09 TIME- 09:49

N30 ; TOOL - 1 DIA. OFF. - 0 LEN. - 1 DIA. - .125 DRILL/MISC ) N30 M25 G49

N40 G0 G90 G20 G17 G40 G80 G90

N50 G28

/ N60 G91 G28 Z0.

/ N70 G28 X0. Y0.

/ N80 G92 X10. Y10. Z10.

( TEST )

N90 T1 M6 ; DIA. - .125

N100 S0 M5

N110 G0 G90 X0. Y0. A0.

N120 G43 H1 Z.238 M7

N130 G99 G81 X0. Y0. Z.123 R0. F.5

N140 G80

N150 M5

N160 M9

N170 M25 G49 H0

N180 G28

N190 A0.

%

Z rapids to Z.238 and is meant to feed down to Z.123 however after getting to Z.238 Z is rapiding to Z0 (center of my part) OUCH then feeding UP to Z.123.

Anyone got any ideas why. Kept this test program as simple as possible so am pretty sure it is not my clumsy programing.

Oh yeah thoes 3 lines of code with the slah. where did they come from??? i have ben deleting them before i run the program but in this sample i left them in if they give you any ideas

[Mike Whitten CAD/CAM Contractors]

The Z is rapiding to Z0 because of the R0. in the drill cycle line. This R value must be set to slightly above the top of the surface you are drilling. It is easiest to use incremental(in the MC op edit:/assuming the geometry is in the correct location) with a value of about .03-.10

 

The G92 is most likely coming from an mi setting. Open an op and look at the misc integers.

 

Mike

 

[ 04-19-2009, 01:34 PM: Message edited by: Mike Whitten CAD/CAM Contractors ]

[buck30]

thanks mike. I should add that i am using a flat pattern then using axis subsituation in Y coming up with this program so i am not using a solid model to get the geometry. Some day i got to learn how to do this though. yeah having one frustrating work weekend here.

 

good to see i wasn't going mad compleatly, was looking far a Z0 line but i see that R0 does the same thing

[Mike Whitten CAD/CAM Contractors]

Glad your running again.

[Justin Beebe at Folsom Tool]

buck30

 

To me it appears that your retract is set to an absolute value of 0. The rapid move to Z0 is coming from the R value in your drill cycle. Try changing the retract to .1 incremental and you R will change to a value .1 above your to of stock

[buck30]

thanks Justin where do i go to make these changes??? yep biginner here lol

[Justin Beebe at Folsom Tool]

buck30

 

You need to make these changes on your toolpath parameter page within your drill cycle. If you can share I file I will show you how I would set them

[Hardmill]

Buck you need to change the retract on this page

 

 

 

PEACE

[buck30]

i turn off the clearence make the retract like .1 (can't remmenr if it ABS. or INCR. wotever the default is) top of stock .000 and depth -.015 put a positive value of the radous so the Z axis knows where Z0 is. Have done this for a few years on these same parts, always worked till this weekend. this is why i am pretty sure some setting change that got done in the name of the new machine is my problem.

 

so on the above test program the radous of the part is .138 , Z rapids it .1 of the top (.238) and center drill .015 deep (.138-.015= .123)

this is wot it is meant to do anyway.

thanks for all your help out there guys. would love to go in early in the morning and get this done.

[Justin Beebe at Folsom Tool]

What value do you have for top of stock. I beleieve when you select rectract of .1 incremental the incremental move is .1 above the value you have entered for top of stock. For example:

 

Top of stock is Z = 1.00

Retract is .100 incremental

Your R value will be Z = 1.100

 

Also why do you turn off the clearance?

[buck30]

top of stock is 0.0 I offset the center of the part by the radous in the Z offset. I know this is not the real way to do this but is the way i wasshown way back when and have done it all this time.

 

turn off the clearence as i have nothing to clear in this case. And trying to make this test program as simple as possible

[buck30]

i should also add that the machine i am using is an old retro-fit knee mill. So i reset the Z height with every job as the knee is moved. i hope this makes sence.

[Justin Beebe at Folsom Tool]

So it sounds like you would want:

 

Z origin should be 0.00

Top of stock should be .138 absolute

Reract should be .100 incremental

Depth should be .123 absolute

 

I would also use clearance of 1.138 absolute

 

Try those settings

[buck30]

ok thanks justin will give it a whirl early tomorrow.

[buck30]

ok here at work now and still rapiding to z0. It is that R0 code that is giving me problems for sure. how does one get that to change????

[Hardmill]

Change your retract to .1 and make sure

its absolute. Look at the pic i posted.

 

 

PEACE

[buck30]

ok got it sorted. YAAAAAA for Jimmy my MC guy in Phoenix. aparently there is a bad but very similar post still deep back there somewhere, the Methods guy aparently loaded the little bit bad post which worked up till i used rotary axis.

Thanks guys for all your help, no doubt you be hearing form me again with my next crises