Contour a circle

[Thad]

When contouring a circle to finish it's wall, I want to use cutter comp AND start at the circle's center point. Can this be done? I wasn't having any luck with "use entry point."

 

Actually, I would like to start at the center, do a straight move perp to the arc turning comp on, cut the arc, and do a straight move perp to the arc going back to the center point turning comp off. Just like you would program it manually with G code. I realize, ideally, I would ramp on to the arc. In this situation, a perp move on is fine. Because of the way the machine handles cutter comp, I need to start and end at the center of the circle.

 

Thanks.

Thad

 

[ 05-23-2002, 09:11 AM: Message edited by: thad ]

[Guest]

Go to toolpaths, next menu, circ tlpths, cricle mill.

[ChrisD]

Hi Thad,

 

You can draw a point in the center of the circle

then Toolpaths--contour---then pick the point first and then chain the arc. In lead In/ Lead out

make sure everything is set to zero and check off the use entry and use exit points.

 

chris

[Trevor Bailey]

If using the entry point method is not working for you, create a point at the center of the arc. There are a couple of ways of doing this. Add the point to your gemoetry if you have an operation already. Simply tell MC to start at the point first, then select the round geometry you wish to machine. Leave the "start at entry point" on. Everything should work fine.

[Thad]

Thanks for the replies.

 

Marc - circle mill doesn't seem to allow cutter comp.

 

Chris and Trevor - you guys kind of had the same response. I still didn't get it to work. I got errors saying to check my radius sizes and entry and exit lines. I selected to use a perp line entry and exit only...no arcs. I'm cutting a .811 dia with a 1/2 end mill. Any more suggestions?

 

Thad

[kccadcam]

In circlemill you have to set entry,exit arc sweep to less than 180, that way it will put a small line for lead in/out so cutter comp will work. I've set mine to 120 degrees and never had a problem with cutter comp. The ONLY way to go for Cbores and such.

[Keith Graydon]

OK Here is one of my really big programming secrets... ok so its not that big.....

 

To arc in and arc out of a bore when starting at its CENTER, do this, given the following.

 

1.25 in dia bore

 

.500 dia. cutter

 

type the following formula into the RADIUS field of the leadin/leadout ARC option.

 

(bore diameter-tool diameter)/4

 

then press enter.

 

use 180 degree arc.

 

press the arrow button in the middle of the dialog to autofill the arc out fields with the same info

 

see image below

 

cutter comp should initiate with the first arc move towards the bore.

 

 

HTH

KLG

[Jack K]

This is the way I like to do it for our Okumas which are a pain for cutter comp. Toolpaths-countour-point... (pick center)then outside of circle. In lead in & lead out pick perpendiclar of entry & exit... check use enrty point & use exit point. No values of checks in any other box.

Works for me.

 

jk

[Thad]

Kevin,

 

The circle mill option seems a little different. Where do you define the tool being used? It cuts the inside of the circle but I see no options for cutter comp. The posted program has no G41 either. Is this something that has to be manually editted? Also, to view the parameters, it points me to an .NCI file. I don't get it. I guess you can tell I'm new at this.

 

Thad

[cadcam]

Thad are you doing what trevor and Chris are saying and along with the point make sure Lead in an out is on and in the box make sure the "use entry point " is checked along with the standerd info of "line""Arc" entry and make sure that you have the point fisrt if you ad the point after all ready have paths.

 

I do this all the time.

you are using at least 8.1.1 correct?

thanks jay

 

[ 05-23-2002, 10:44 AM: Message edited by: cadcam ]

[kccadcam]

Thad, what version of MCAM are you using???

[Thad]

Jack,

 

Could you try that with a .811 dia hole and a 1/2 dia endmill? I did that and got errors.

 

Thanks.

Thad

[cadcam]

thad is this what you want it to look like?

 

%

O0000 (T )

(23-05-02 -07:44 )

G0 G40 G49 G80 G90

T1 M6 ( 3/8 FLAT ENDMILL )

A0

G0 G90 G54 X0. Y0. S1426 M3

G43 H1 Z.25

Z.1

G1 Z-.5 F6.33

G41 D1 X.0625 Y-.0187

Y0.

G3 X-.0625 I-.0625

X.0625 I.0625

G1 Y.0187

G40 X0. Y0.

G0 Z.25

M5

G91 G28 Z0.

G90 G49

G53 Y0

M30

%

[Thad]

V7.2c

 

We have v8.1, but I was trained on 7.2 and I'm more concerned with getting work out on the floor than dealing with the v8 "issues" my trainer told me about. For right now, anyway. See "v8 issues" thread for a little more history on this. Perhaps v7.2 is my problem???

 

Thad

[Thad]

Jay,

 

Yes, I've done what they said. The point is the first chain, then the circle. I have use entry point and use exit point selected and I've tried all zeros for the entry and exit moves along with various values. I get the same errors that say to check my radius sizes and entry and exit moves no matter what size line or radius I use.

 

Thad

[kccadcam]

Version 7 was still a chook, version 8 it is under toolpaths,next menu, circ toolpaths, circmill.

Thats why your having problems.

 

This is what I get using circlemill the way I told you in V8 or V9.

BTW, V9 is the only way to FLY!!!!!

 

.5 tool with .75 bore

 

%

O0010

(CUSTOMER - )

(PART NO- REV- )

(PROGRAM NAME - TEST )

(DATE=DD-MM-YY - 23-05-02 TIME=HH:MM - 08:59 )

( TOOL - 3 DIA. OFF. - 33 LEN. - 3 DIA. - .5 1/2 FLAT ENDMILL )

 

G20

G0 G18 G40 G49 G80 G90

( TOOL - 3 DIA. OFF. - 33 LEN. - 3 DIA. - .5 1/2 FLAT ENDMILL )

( CIRCLE MILL )

T3 M6

G0 G90 G54 X1.281 Y0. S5000 M3

G43 H3 Z.1 M8

G1 Z-.5 F50.

G41 D33 X1.3123 Y-.0541

G17 G3 X1.3435 Y-.0625 R.0625

X1.406 Y0. R.0625

X1.281 Y.125 R.125

X1.156 Y0. R.125

X1.281 Y-.125 R.125

X1.406 Y0. R.125

X1.3435 Y.0625 R.0625

X1.3123 Y.0541 R.0625

G1 G40 X1.281 Y0.

G0 Z.1

M5

G91 G28 Z0. M9

G28 Y0.

M30

%

[cadcam]

Ok this what I get on the screen in ver7

 

hee is the screen shot.

[robyyz]

thad, to keep it simple I would only select the circle as your geometry, and use the lead in/out to control where the toolpath starts. Your lead in/out should only consist of a line, you should select perpendicular, your line length should be half of your diameter (ie. 0.811 / 2). Make sure to put this value in the second box...first box, percentage should be 81.1. I find picking a starting point sometimes gives extra values in the NC output and confuses the controller.

 

Rob

[Keith Graydon]

or do you want it to look like this?

 

posted for FADAL.

 

.811 bore. .500 cutter, climb cut, arc in, arc out, FROM CENTER, With G41. twice around with finish cut.

 

=================================

TA,1

%

N1O0000(bore)

N2G0G17G40G49G80G90H0E1Z0

N3T1M6(DIA. - .5)

N4G0G90S2200M3E1X-.005Y0.

N5H1Z2.

N6A-0

N7Z.1

N8G1Z-.25F4.

N9G3X.0727Y-.0778I.0778F6.5

N10G41D1X.1505Y0.J.0778

N11X0.Y.1505I-.1505

N12X-.1505Y0.J-.1505

N13X0.Y-.1505I.1505

N14X.1505Y0.J.1505

N15X.0727Y.0778I-.0778

N16G40X-.005Y0.J-.0778

N17G0Z2.

N18X0.

N19Z.1

N20G1Z-.25F4.

N21G3X.0778Y-.0778I.0778F6.5

N22G41D1X.1555Y0.J.0778

N23X0.Y.1555I-.1555

N24X-.1555Y0.J-.1555

N25X0.Y-.1555I.1555

N26X.1555Y0.J.1555

N27X.0778Y.0778I-.0778

N28G40X0.Y0.J-.0778

N29G0Z2.

N30M5

N31M6

N32E0X0Y0

N33M30

%

 

KLG

[Jack K]

Thad,

 

I tried it with a .811 circle and a 1/2 end mill and it seem ok to me. The code also looks good.(PROGRAM NAME - TEST)

(DATE= 23-05-02 TIME= 10:13)

G90G80G40G0

T23M6(.500 MILL )

G15

G0G90X0.Y0.

S600M3

G56H23Z1.M8

Z.1

G1Z-.2F5.5

G41D23X.4055

G3X-.4055I-.4055

X.4055I.4055

G1G40X0.

G0Z1.

M9

G30P1M5

G15H0X-18.Y10.

M30

%

 

Jack

[kccadcam]

Ok, Here is the formula you are looking for:

 

Hole dia. - cutter dia./2 = offset distance

This is the main value you have to know.

 

here it get a bit more compliated, so bear with me.

 

1/squareroot of 3 * offset distance = Lead in/out

 

offset distance/3 = Arc radius

 

Arc sweep is ALWAYS 120 deg.

 

expamle. 1 1/2 dia hole with 1/2 e.m.

 

1.5 - .5/2 = .5 <---.5 is the "offset distance"

 

1/squareroot of 3 * .500 = .28867 = lead in/out

 

.5/3=.166666666666 = Arc radius

 

Arc sweep = 120 deg.

 

oh, yes, the 1/squareroot of 3 number I have been talking about is equal to .57735

 

Thanx to my programming partner in crime, James Cook

 

[ 05-23-2002, 11:39 AM: Message edited by: kccadcam ]

[cadcam]

Thad I emailed you a MC7 file with a .811 dia hole and a .500 em.

 

Hope this helps.

[ROB]

leadin/out

check- entry exit

select perpendicular- entry exit

lenght=size of circle minus dia of cutter

divide by 2- entry exit

ramp 0 -entry exit

radius=size of circle minus dia of cutter

divide by 2 -entry exit

sweep 0

helix 0

 

should start at center and finish at center with

c/comp on

 

try it...

[James Cook]

to elaborate on my above forumla using your example of .811 dia hole with a .500 e.m.

 

Lead in/out=.089777966

 

Arc radius= .051833333

 

Arc Sweep= 120 Deg.

 

Works every time...also can be useful for other things too.

 

EDIT---also must use tangent entry for this to work

 

[ 05-23-2002, 01:51 PM: Message edited by: James Cook ]

[Thad]

"Version 7 was still a chook, version 8 it is under toolpaths,next menu, circ toolpaths, circmill.

Thats why your having problems."

 

Good try Kevin, but that's not it. Circle mill is located where you just said, I just get errors doing it. Oh well, I'm off for the weekend so I'll have to try again on Tues. Thanks you for all your help and have a nice, safe Memorial Day weekend!

 

Thad