Need Help!- using cutter comp in tights pockets/slots

[GM81]

I am having some issues using cutter comp to finish a tight slot. First off I am using Mastercam XMR2

I have a part that requires 3 .250 +.002 -.000 slots cut into it. I am using a 7/32 EM. 2 passes to get it to depth and then I want to finish it using comp. I can't get mastercam to either initiate comp out of the pocket and then finish it, or to move length wise in the center of the pocket to initiate and then goto depth and finish cut.

Any help would be greatly appreciated.

Thanks!

Garrett

[Superman]

Try using 3 operations

op1-Drill- drill 15/64" holes at arc centers
op2-Rough- 2D Contour between arc centers-comp OFF-NO lead in/out
op3-Finish- 2D Contour - pick 1 arc center point then the (nearest entity)chain going CCW for each slot
use---- comp ON ( wear ), lead in/out ( midpoint start/finish OFF, perpendicular, line=0, arc 0.010" , 45°, use entry point ON, copy Left side to Right )

[psychomill]

..... or ......

Moving around the start point of the pocket chain will move around the finish path start points. Typically in a slot, MC does move to the "center area" of a slot where the pass will start. It's just a matter of adjusting your lead in/lead out moves to get it where you want to start those from. Personally, I'd use a smaller endmill then a 7/32 for that size slot but ..... that's me.

As for initiating comp outside of the pocket... your post has to be written or 'switchable' to do that (needs the logic in the post).

Superman offers another method (a little longer to do) but be careful about having "0" line length... many machines aren't set up to comp on an arc start.

[GM81]

I was doing what you suggested superman except in the 3rd op, I was starting at where the arc ended. I am using a Fadal 88 control if that matters. I was thinking the problem was from not having enough room to move 1/2 the Dia of the tool, so the comp was just ignored by the control. I have never had to worry about this before, most parts we work on are a bit larger and there has always been plenty of room.

I guess I could use a smaller tool for a finish pass, I just don't like going smaller than .250 when running steel pieces, its CRS, cuts easy enough. I was trying to stay away from to many tool changes, but I might have to give it a go.

Thanks for the info. I am only self taught at MC, much to learn.

The customer needed 24 pcs by tomorrow morning, so I just created a custom tool in MC @ .216 dia and ran 7/32 to get it done for now. I will try and fix things up when we go to production mid week.

[Superman]

Did you pick the center point of the arc and then chain the contour ?
each slot should have a "chained point" before the "chain"

use---- comp ON ( wear ), lead in/out ( midpoint start/finish OFF, perpendicular, line=0, arc 0.010" , 45°, use entry point ON, copy Left side to Right ) D value in the machine set to zero
use---- comp ON ( control ), lead in/out ( midpoint start/finish OFF, perpendicular, line=0, arc 0.120" , 45°, use entry point ON, copy Left side to Right ) D value in machine set to tool radius or diameter depending on your machine


The tool will rapid to the chained point and descend on that point to depth and will take up comp on a line ( and then arc lead in ), then go around the chain

Is that a bit clearer ?

[psychomill]

missed the chained point.... should work.
The Fadal requires to move "1/2 the diameter of the tool" to take up comp?

[GM81]

I used the center point of the arc before the chain, but I come into the flat and lead out at the end of the rad.

I thought all machines required a move of 1/2 the dia. to initiate cutter comp?

[psychomill]

No. That was the suggested procedure way back in the day along with first comp move to be perpendicular to the first cutting direction. But it's not so anymore unless you have a super old control. However, if you centerline program, then yes... you need at least 1/2 the diameter. It has to do with the math for wear. If your wear value exceeds the distance of the comp take up, most controls will alarm out.

EX: 1/2" tool, .250 in the wear, Lead In comp move is only .100 = ERROR.

One of the benefits of programming using tool edge is you can now run in real tight spots and avoid many (inside) arc alarms from additional comp needed based on the tool values and the part program. You can do a .001 lead in move if wanted to. Same rules of math applies though... As long as the comp doesn't exceed the value of the lead in motion or you overcomp the tool based on part geo.

[GM81]

It must be the control then, for a majority of my machining career I have been on Fadal 88 controls, hence why I thought that was a standard.

Thanks for the info, it appears I am SOL on this for now, but a good learning experience.

[psychomill]

Haven't been on a Fadal in 20 years so I don't remember much of the comp restrictions....

But I wouldn't think you're SOL... Just have to work with the way you're doing it. Superman made some good points and examples... I'm sure you'll find your way....

[Superman]

Originally Posted by psychomill However, if you centerline program, then yes... you need at least 1/2 the diameter. It has to do with the math for wear. If your wear value exceeds the distance of the comp take up, most controls will alarm out. EX: 1/2" tool, .250 in the wear, Lead In comp move is only .100 = ERROR. One of the benefits of programming using tool edge is you can now run in real tight spots and avoid many (inside) arc alarms from additional comp needed based on the tool values and the part program. You can do a .001 lead in move if wanted to. Same rules of math applies though... As long as the comp doesn't exceed the value of the lead in motion or you overcomp the tool based on part geo.

I think there is some confliction here in what you are stating
Please consider that we are machining around the inside of a rectangle

In Mastercam,
CONTROL will output a toolpath that is only offset from the rectangle lines by the amount you allow in the XY allowance.
If lead in/out is chosen, it must meet the requirements of your machine, many require that a linear mode is used to take up compensation ( climb milling means using a G41 or LEFT comp ), we usually make the descend in point more the the tool radius away from the start of the contour to minimise dwell marks down a wall or overcutting ( tool wobble ) when plunging into material. The tool will move from it's descend in position to take up the comp and be perpendicular to the start point ready to go to the next point in the chain. It could cross itself to take up comp
The idea of programming to CONTROL is it also allows you to use a still smaller tool with no change to the program, just alter the machine's D value for that tool. The tool comps reflect the actual tools used

WEAR will output a toolpath that is offset by the tool radius plus the XY offset allowance you have permitted ie 1/2" tool and 0.010" offset will give a toolpath that is offset by (1/4"+0.010"=) 0.260"
In this case you set the tool radius in the machine to zero if you use a 1/2" tool, you can use + or - values for the D comp, + means stay further away from the profile, and - means cut closer to your desired profile.
ie 1/2" tool and 0.010" offset will give a toolpath that is offset by (1/4"+0.010"=) 0.260", if D comp =0 then 0.010" wil be left on the wall, but if I dial in -0.010" then the cutter has negated my XY allowance and actually finished the wall
If lead in/out is chosen, remember you are now programming the tool centre line and D comp is 0 , lead in/out values can your choice, but ideally large enough to allow you to adjust in the machine ie, a 0.02" line lead in and out allows you maximum +0.02" tool comp , a (-ive tool radius) comp will make the tool travel on your profile

Tool comps, if all tools are as programmed, would be set to 0(zero)

Wear assumes that the same diameter tools will be used next repeat of the job, if the tool happens to be re-sharpened, then a -ive comp would be used to make the tool cut closer to the part ie 1/2" tool re-ground to 0.460" then a -0.020 comp would be dialed in.
formula
( actual tool dia - programmed dia ) / 2 = D offset to dial in
===== ( 0.46 - 0.50 ) / 2 = -0.02

Using larger tools than what was programmed has some dangers and must be checked properly ( descend points may be in the wrong area, inside arc may be smaller than the tool radius, etc)



Boy, what an essay, I need a drink

[psychomill]

... make that two drinks...

I thought that's what I was saying but perhaps overly simplified and I didn't get into the particulars enough as you did...