OffSet?

[CharlieM]

I wrote a short program to go over .375 to a starting point, plunge down .125
with a .062 end mill, then go up, across, down, and back to start, retract the mill and go home leaving a .313 wide by .438 high window with .03 radius at the corners. Is there a way to make the window .323 wide by .448 high by setting a .005 offset? What would it look like in my program below?

Any help is much appreciated.

Charlie


G00 X.375 Y.000
G01 Z-.1250 F.75
G01 X.375 Y.375
G01 x.625 Y.375
G01 X.625 Y.000
G01 X.375 Y.000
G00 Z.0000
G00 X.0000 Y.0000
M30

[Geof]

Yes but first you have to put in the tool compensation command; G41 or G42 with the D address that has your 0.005 value. Actually depending whether your machine uses radius or diameter for tool size you may need 0.010.

Your rapid move to the start position will be: G00 G41 D? X.375 Y.000

At the end the rapid move will have G40 to cancel tool comp.

[CharlieM]

Can't make it work like that. When I try to load the G41 offset value the machine goes directly to the second address (G01 X.375 Y.375) and ignores the .005 offset, ruining the little window!

I never use tool radius, I program tool path and let the tool path account for the tool radius. In this case the tool is a 1/16 Dia. endmill and the tool path is 1/16 smaller than the window that I am cutting.

This is a home-built mill and the program that I am running is "Master 5".

[HuFlungDung]

Radius compensation is not quite that simple. You have to preplan what we call a lead-in and a lead-out to the profile. This means that you deliberately send the tool to a start position that is the comp radius away from the profile. Now, when you turn comp on with G41/G42, the controller can shift the tool from center to edge on the profile (without a visible movement) and thus prevent the spoiling of the profile.

Some old controllers did actually execute a movement when comp was turned on. But, most modern controllers combine the comp value with the first movement, creating a net vector that puts the tool edge tangent to the profile.

So what you could do, is break one side of your square in half, and add a lead-in line from there to the geometric center of the square. Also, add a lead-out line from the profile back to the center to get the tool clear of the profile when turning comp off.

[Geof]

Originally Posted by HuFlungDung Radius compensation is not quite that simple......

On a Haas it is. Provided the first move is greater than the tool radius entry; in other words move from X0. Y0. to X.375 Y0. is plenty far enough. Similarly the move back to X0. Y0. at the end is enough to cancel.

[HuFlungDung]

Yes, Geof, I suppose it is, but how often is it desirable to have the tool descend to cutting depth right on the finish profile?

[Geof]

Originally Posted by HuFlungDung Yes, Geof, I suppose it is, but how often is it desirable to have the tool descend to cutting depth right on the finish profile?

Given that the code without tool comp was doing this I figured doing it with would be no different.

[psychomill]

I agree with Geof... It is simple. As long as the amount of lead in is longer than the amount of comp, it works fine. Although on some machines, it will try take up comp even though the comp is greater than the "lead in". Not many will try, but some.

Additionally, I also agree with Hu. Dropping in Z at the finish profile will often leave a mark on the profile. Now in this case, he's dropping into the corner of a small window with a small endmill, so the witness mark in this case is probably next to none. But often times, you could end up with a mark on the profile. I (as probably Hu) prefer to take up comp in this example with something like this:

G00 X.580 Y.100
G01 Z-.1250 F.75
G01 G42 D?? X.580 Y.05
G01 X.500 Y.000
G01 X.375 Y.000
G01 X.375 Y.375
G01 X.625 Y.375
G01 X.625 Y.000
G01 X.450 Y.000
G01 X.400 Y.050
G01 G40 X.400 Y.100
G00 Z.0000
G00 X.0000 Y.0000
M30

This way, you take up comp before entering the finish profile. Notice in this case I used G42. If you're cutting a window and your spindle rotation is normal direction, then according to your code you're conventional cutting. So in order for .005 comp to take effect, you need G42. In your D offset, you would have a -.005 to "overcut". Keep in mind, since you're not using a radius in the corner movement, your window will be larger but your corner radius will remain .03 .

Additionaly, for this case, you could use a G41 and still make this happen. Just use a positive comp at .005 and it will cut the same. But that is not the norm since you're "lying to the lie" to the machine if you get my drift.

Further note: I don't know anything about a "Master 5". This is based upon FANUC type or ISO code controls. I know there are a couple of home built mill type software that doesn't accept comp or has some additional movements needed in order to take up comp.

[CharlieM]

Thanks Psychomill, cutting that window has turned out to be more difficult than I expected. You are right, I should have been clinb milling instead of conventional milling. I will load this program and test it, but what do I put as the value for D??. My End Mill is 1/16 Dia.

Master5 is a simple program that is no longer available, (it has been upgraded several times) I have downloaded the newer versions but cant make sence out of them.

I have tried to use K-Cam but can't make the (F) command work for feeds.

[psychomill]

but what do I put as the value for D??.

That's the part I'm not sure about since I'm not familiar with your control software. On a commercial CNC though, the "D" represents the offset number to be used to control the amount. On CNC controls that I use, there is a numbered tool offset page. Since most machines have tool storage and tool changers, the offset page allows you to set the tool length and diameter offset. For example, the endmill is (in your case 1/16) Tool 1. So you store the tool length at offset "1" on the offset page. For cutter comp, you might designate offset number "21". In 21, you place a -.005 as the value. Then in the program, you use "G41 D21" to pick up the comp value.

Hope that helps. If the software you use can't accomodate the use of tool offsetting, then you'll have to reprogram your window, hard numbering the tool comp by programmed position.

Additional note: The program example I wrote is just an expanded program you wrote. That program is still conventional cutting...

[CharlieM]

If I want a .005 finish cut I will run this program first.

G00 X.380 Y.005
G01 Z-.1250 F.75
G01 X.380 Y.370
G01 x.620 Y.370
G01 X.620 Y.005
G01 X.380 Y.005
G00 Z.0000
G00 X.0000 Y.0000
M30

I was hoping there was an easier way.

[ajl6549]

Try this:


G00 G41 D?? X.625 Y0
G01 X.375 Z-.1250 F.75 (ramp z down)
Y.375
X.625
Y0
X.375
(2nd, if ness.
Y.375
X.625
Y0
X.375)
G00 Z.0000
G40 X0 Y0
M30

This should leave a minimal entry/exit line. If you need to you can go around twice if ness. to relieve tool pressure