[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]

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]

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

[Geof]

Once you have this program running and doing what you need go onto the next step and use G91 G03 I J Z-z L where -z is the amount you helix down on each interpolation.

For instance your 0.25" high boss would need G91 G03 I J Z-.05 L5 to helically interpolate down 0.25".

You then follow with a final interpolation in absolute to remove the last helical ramp so the full program is:

G01 G41 D01 X Y Z F (where X Y Z puts you at the top of the boss and at the correct radius)
G91 G03 I J Z-.05 L5 (this helically interpolates down the boss)
G90 G03 I J Z-.25 L2 (this cleans up the ramp at the bottom and the L2 gives a spring pass)
G01 G40 X Y Z (cancel tool comp and move away)

[stevespain]

hi everyone, new to the site hope to get involved with discussion ....

[mactec54]

glenthemann

capitalcrew wanted a program he could run/cut his part with, to do this you need to know the tool/EndMill size

[Geof]

glenthemann

capitalcrew wanted a program he could run/cut his part with, to do this you need to know the tool/EndMill size

Provided the tool diameter is in the correct entry in the tool diameter offset table you do not need to mention it in the program and the programs restrictions are; any compensation moves must be greater than the tool radius and any internal radii and straight moves between corners in the program must be larger than the tool radius.

He does mention above that he has the diameter and length in the machine.

[mactec54]

Hi Geof

Not correct,The tool is not mention in the program I did for him, to make him a new program using a cam program you have to have the the tool size, you put this imformation in the cam software, you then don't have to mess with the program if you have this imformation

Hand programing you don't need the tool size like you have said,you call it out from the tool offsets,& just do you tiwittering
& hope everything is right or crash

[Geof]

What he had in his first post didn't look like CAM output to me. Was it?

[glenthemann]

You need to know the tool size if youre not applying any cutter comp. I did not actually look at your program to be honest, and if you didnt use comp in it then yes you are correct, youd need the tool size.

However like I said, using comp (which I assumed threadstarter wanted to do seeing as he had a D value in his original post), you do not need to know the tool diameter right off the bat. we know the hole size, so just send your comp apply move to distance of the hole just to save headaches and make programming easier on yourself. The distance can always be made shorter later on once a tool size is established. Better yet you can use a bit of macroing to have the machine choose the comp distance based on the D offset.

I hate not using comp now, it frustrates the hell out of me and the other programmer in my shop hates using comp. On some simple parts Ill program without comp, but on the critical areas ill use a user parameter and set it as my "comp" parameter. Ie. if I have to mill out a flat along x1.0, ill command the move as g1 X[1.0 + P1] and use the P1 value as the tool wear.. works for simple programs. But in my opinion you should always try to use comp. It may take a little longer initially but will save you loads of frustration and headaches in the long run.

Even camming something out can be slower. Oh no you dont have another 1/4" endmill around and only have a 3/16? damn, guess you have to go back into cam, change everything, re up the data to the machine, verify etc. Worse yet, at my work the other guy will only cam out a specific section or profile of a part at a time, print it out and manually enter all the new code. Then hell get mad at me for "taking so long" to code something out, or come over and be like "wtf youre using full diameter values" (if he does use comp he'll still program as if there is no comp and use a 0 diameter value..)

I dont get what you mean by "hand programming you dont need tool size"

really? you can hand program with, or without comp, and infact its easier initally to program without comp (saves you comp apply moves, you can move back and forth witht he cutter without having to come off the part, turn off comp, reapply to other side etc) and in that case you actually would need the tool size. Not bashing you or anything, dont get me wrong, I just dont quite understand where you're coming from mac.

Anyway, I think the threadstarter should be good to go now

[capitalcrew]

%
O04401 (part 44 side 1)
T1 M06 (LOAD ENDMILL)
G90 G54 (ABS OFFSET)
G43 H01 (TOOL LENGTH TOOL#1)
M03 S300 (SPINDLE ON 300 RPM)
G00 X0 Y0 (RAPID TO ORIGIN)
G01 G41 D01 X2.0 f4.0 (feed TO PT#1)
G00 Z0.1 (RAPID TO R-PLANE)
M08 (COOLANT ON)

G01 z-.050 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 g40 (clear part)

G01 x2.1 z-.1 f4.0 g41 d01 (feed down .1)
G01 x.3438 f4.0 (move over to edge of circle)
G02 I-.3438 J0.0 (circle clockwise)
G01 x2.0 g40 (clear part)

G01 x2.1 z-.15 f4.0 g41 d01 (feed down .15")
G01 x.3438 f4.0 (move over to edge of circle)
G02 I-.3438 J0.0 (circle clockwise)
G01 x2.0 g40 (clear part)

G01 x2.1 z-.2 f4.0 g41 d01 (feed down .2)
G01 x.3438 f4.0 (move over to edge of circle)
G02 I-.3438 J0.0 (circle clockwise)
G01 x2.0 g40 (clear part)

G01 x2.1 z-.25 f4.0 g41 d01 (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 g40 (clear part)

G00 Z1 m09
Z0 M05

M30
%

Leaving cutter comp on after each circle was giving me rectangles around the part, it doesn't do it if I turn it on and off for each operation. I'm just posting this to show you guys where I'm at, and I'm going to try it helixing down. I'll post that when I've finished it. Should only be a few minutes. I'll try both when I get a chance to use a machine, we only have three mills so I have to wait for some one else to finish.

I made a few changes at the machine yesterday, so I might have forgetten to put those changes into this as well.

Oh, and no I am not using any software to do this. I'm writing it by hand, in microsoft notepad.