Need Help!- I can't get this program to work right

[capitalcrew]

I'm pretty new at this and I need to circular interpolate an 11/16s diameter boss on a small eccentric shaft. It will be .250 high when it's done. I have gotten it to graph on a haas TM1, and it does run, but it doesn't look like it is doing what I need it to do. The teacher of this class isn't much help, and I need to finish this today. If anyone can get back to me asap I'd really appreciate it.

I really only need one block of it to be right, then I can make the rest the same just with a different depth for it to feed down. Go easy on me guys.. lol


%
O04401 (part 44 side 1)
T1 M06 (LOAD ENDMILL)
G90 G54 G41 (ABS OFFSET CC ON LEFT)
G43 H01 (TOOL LENGTH TOOL#1)
M03 S300 (SPINDLE ON 300 RPM)
G00 X0 Y0 (RAPID TO ORIGIN)
G00 X2.0 Y0 (RAPID TO PT#1)
G00 Z0.1 (RAPID TO R-PLANE)
M08 (COOLANT ON)

G01 z-.050 D01 f4.0 (feed down .050)
G01 x.3438 f4.0 (move over to edge of circle)
G02 I.3438 J0.0 (circle clockwise)
G01 x2.0 (clear part)

G01 z-.1 D01 f4.0 (feed down .1)
G01 x.3438 f4.0 (move over to edge of circle)
G02 I.3438 J0.0 (circle clockwise)
G01 x2.0 (clear part)

G01 z-.15 D01 f4.0 (feed down .15")
G01 x.3438 f4.0 (move over to edge of circle)
G02 I.3438 J0.0 (circle clockwise)
G01 x2.0 (clear part)

G01 z-.2 D01 f4.0 (feed down .2)
G01 x.3438 f4.0 (move over to edge of circle)
G02 I.3438 J0.0 (circle clockwise)
G01 x2.0 (clear part)

G01 z-.25 D01 f4.0 (feed down 1/4")
G01 x.3438 f4.0 (move over to edge of circle)
G02 I.3438 J0.0 (circle clockwise)
G01 x2.0 (clear part)

G00 Z1 m09
G40
Z0 M05

M30
%

[mactec54]

capitalcrew

You don't say what size tool you want to use

[capitalcrew]

I have the diameter set on the machine and the length is in the machine also. It says D01 for the diameter of tool 1

[mactec54]

capitalcrew
Nobody can make you a program with that imformation what is the dia of the endMill you are using

[capitalcrew]

I wasn't asking for anyone to make me a program I was just asking if anyone saw anything wrong with the one I have.


The diameter of the endmill is 1.165, it is a 6 flute endmill. I want the center of the circle to be the origin.

Thanks.

[guru]

"I" should be negative (G02 I-.3438 not unless your control takes absolute I and J0).

Move G41 to (move over to edge of circle) block

Add G40 to G01 x2.0 (clear part) block

.....Try that first

[JWK42]

"G01 z-.050 D01 f4.0 (feed down .050)
G01 x.3438 f4.0 (move over to edge of circle)
G02 I.3438 J0.0 (circle clockwise)
G01 x2.0 (clear part)"

I think after a quick look you need to have a I-.3438 in your G02 line
I believe the rule is "Distance and direction from the start of the arc to the center of rotation."

Comment--

I see Guru posted while I was writing this. I agree with his answer

[mactec54]

capitalcrew
This program will rough cut all the way done in .06 steps & then do a clean up pass around the part no D01 needed in the program, just save the program & put it in the machine, it has the same program number as you had plus same speed & feed
There is no G40/G41 if you want need to have cutter comp it will have to be added to the last operation

[beege]

Originally Posted by capitalcrew I'm pretty new at this and I need to circular interpolate an 11/16s diameter boss on a small eccentric shaft. It will be .250 high when it's done. I have gotten it to graph on a haas TM1, and it does run, but it doesn't look like it is doing what I need it to do. The teacher of this class isn't much help, and I need to finish this today. If anyone can get back to me asap I'd really appreciate it. I really only need one block of it to be right, then I can make the rest the same just with a different depth for it to feed down. Go easy on me guys.. lol % O04401 (part 44 side 1) T1 M06 (LOAD ENDMILL) G90 G54 G41 (ABS OFFSET CC ON LEFT) Save G41 for later G43 H01 (TOOL LENGTH TOOL#1) M03 S300 (SPINDLE ON 300 RPM) G00 X0 Y0 (RAPID TO ORIGIN) G00 X2.0 Y0 (RAPID TO PT#1) G00 Z0.1 (RAPID TO R-PLANE) M08 (COOLANT ON) G01 z-.050 D01 f4.0 (feed down .050) Take out the D01, goes with comp. G01 x.3438 f4.0 (move over to edge of circle) Put G41 D01 G01 x2.0 (clear part) and G40 here G01 z-.1 D01 f4.0 (feed down .1) Take out D01 G01 x.3438 f4.0 (move over to edge of circle) G41 D01 here G02 I.3438 J0.0 (circle clockwise) G01 x2.0 (clear part) G40 here G01 z-.15 D01 f4.0 (feed down .15") Take out D01 G01 x.3438 f4.0 (move over to edge of circle) Put G41 D01 here G02 I.3438 J0.0 (circle clockwise) G01 x2.0 (clear part) G40 here... etc. G01 z-.2 D01 f4.0 (feed down .2) G01 x.3438 f4.0 (move over to edge of circle) G02 I.3438 J0.0 (circle clockwise) G01 x2.0 (clear part) G01 z-.25 D01 f4.0 (feed down 1/4") G01 x.3438 f4.0 (move over to edge of circle) G02 I.3438 J0.0 (circle clockwise) G01 x2.0 (clear part) G00 Z1 m09 G40 Z0 M05 M30 %

Corrections in-quote. G41 is usually instituted on the block before your profile starts, at least one tool radius away from the geometry, and turned off again when the geometry is complete. If you don't turn it off, you may get unexpected results. What controller/machine are you using?

[capitalcrew]

I figured out the cutter comp and d01 stuff, and changed it. I tried making the I value a negative and it didn't graph on the machine. I'm using a Haas TM1, I'm guessing the controller is the panel that has all of the controls on it haha. I'm not sure what it is, it came with the machine I believe.

[capitalcrew]

I just tried your program, mactec. It graphes niceley, I'm out of time to run it today though so I will give it a try tomorrow. If it works I'll be back to let you know. Thanks guys for everything so far!

[glenthemann]

Originally Posted by mactec54 capitalcrew Nobody can make you a program with that imformation what is the dia of the endMill you are using

tool dia shoudlnt matter except for the lead in move on comp, must be larger distance away than the radius of the tool.. so just make some big value the size of the hole that way there is no way the lead in move would be smaller than the tool radius.

The problem I see with your initial program is that you are calling D01, but not calling it on a comp initation line G41/G42. Or rather you are not calling any compensation mode at all, so having the D01 in there does absolutely nothing