G99 vs G98 on drill cycle with different "R" Planes

[Matthew]

I'm having trouble with another file. In operation #1 there are 3 different "R" value heights that I'm drilling at. Because of this I have clearance set to .05" ABS, retract set to .05" INC, top of stock set to 0.0 INC, and depth set to -.05" INC. My expectation of these settings is that it will spot drill .050" deeper than every point I have picked while going to an Absolute clearance plane of .050" above the part when it moves XY positions. However, when I post out this code I get a G99 in the drilling cycle which will not allow the machine to retract to .050" Absolute above the part before it moves. If it wasn't caught it would have caused at the least a broken tool, probably a scrapped part etc. If I change the ABS clearance height to .1" ABS then a G98 is posted instead of the G99. This tells the machine to retract to .1" above the part before making an XY move. This is what I want, but it won't work if the clearance value and retract values are the same. I've uploaded a file to the FTP "ROUND_PART.MCX" in the MCX folder. Can someone take a look and see if they get the same results?

 

Thanks.

[Steel Surgeon]

How about Staying all incremental and setting your clearance to .5. This would give you approx 1/8 clearance over the center hub that you would need to clear. Just don't check the box to use only at the start and end of each operation.

[Guest]

Matthew,

 

I placed on the FTP in the same directory

jmparis_round_part.mcx

 

I set up the drills the way that I would do them. Take a look, I think what you are trying to do in one toolpath is going to be difficult. In V9 the toolpath editor would help here.

 

But in X it is not yet available.

 

HTH

[Matthew]

I'll take a look at your file, but I don't think what I'm trying to accomplish is difficult. If I change the value to anything but the .05 in the clearance setting (which is the same as the incremental retract value) then I get the proper output. I used .1 ABS clearance for an example, but I bet .051" would work too. The path backplots fine, and verifies fine, however it outputs the wrong code (g99 instead of g98) which would cause the tool to hit the part.

 

Thanks for the input.

[Matthew]

jmparis,

 

I looked at your file and see what you did by breaking up the operations. However, if I change the clearance value in my one operation to 2.0" I get the same backplot as with what you did. And it posts with the G98. However, the problem with posting a G99 instead of a G98 only seems to appear when the abs clearance height and the incremental retract height are the same value, and it's only the posted output that is wrong. It backplots fine no matter what the value is.

 

Thanks.

[Guest]

I agree, having it set the same .05 does for some reason post out a G99. Changing it to anything but .05 causes it to post a G98.

 

Why,

 

I simply broke those ops up so the G99 would keep the tool down nearer to the flange instead of the 2" retract that I use. It allows me to control when I stay down close to the work and when I clear out of there.

 

Everyone does it different

 

[Matthew]

Thanks Jmparis.

 

I know how to work around it, and I've been doing it since I first came across this problem in V9. I had my default settings to clearance plane .1 and retract plane .05 so it never caused me a problem. However when I started messing around with X I didn't have these defaults set yet and it showed up when I went to run a part. Luckily I noticed it before I started the machine. I thought I would bring it up so see if it's a bug, post issue, or "just the way it is".