Not using cutter comp

[HuFlungDung]

I hate cutter comp. I'd rather redo my code

Anyway, I was pleased to find out that when editing an operation in OnecncXP, that I could put in a negative amount in the "amount to leave for finish" field, and the new parameters will generate the new path with the desired over-cut. This was a 2d style path I was working with.

[E-Stop]

Originally posted by HuFlungDung I hate cutter comp. I'd rather redo my code

Ouch! I ran NC equipment back in the late '70's that did not have cutter comp (or a programmable Z axis, for that matter). Cutter comp is a blessing and I wouldn't want to go back to not having it.

[mlinder]

HU,

How do you adjust for cutter wear? Do you still have G41/G41 in the code so that you can make minute adjustments at the controller?

My 2 1/12 D program (MasterCAM), creates code based on the selected tool diameter. My tool info at the controller (Fagor) is set to 0 offset. When cutting the part, we then, if necessary, change the tool offset by .001 or .002 to adjust if necessary. Leaving G41 or G41 in the code allows me to do this.

Is my way of thinking the "wrong" way? I guess one drawback to programming this way is that if I break my very last "x" diameter tool, I have to go back to MasterCAM and recreate the code for a different tool.

I am sure there are pros and cons to all approaches.

Mark Linder

[Mortek]

For purposes listed, tool wear and size ajustment, Cutter Comp is a wonderful blessing. You just have to understand how it works on your machine. As far as reposting goes, it takes more time to repost than it does to change an offset radius at the control. In OneCnc you can repost rather quickly, but it still takes more time. Approach, depart, path overlap are the things to be concerned about with cutter comp. If you know how to do it you're miles ahead of most. Everyone I know hates cutter comp.. I guess I would say get to know your machines and how they act when given the command. You may find out how wonderfull cutter comp is.

Ken

[wms]

Hu,

BOY DID YOU OPEN A BIG OL CAN OF WORMS

I'm going to get a good laugh out of this post.

Please read my signature!!!

[HuFlungDung]

Ya know, crow tastes like chicken

I know I should learn to use it, but last time I did, the firmware from my controller was acting up, and I haven't bothered to see if they fixed it in the last upgrade.

One thing about OnecncXP, they have really done an incredible job of making the approaches easy to choose and set up. I am tempted to try it one of these days.

I guess that is one thing about using Rcomp before, was doing the approaches so that I wouldn't get accidental gouge when the Rcomp came on. That's why I hated cutter comp.

[E-Stop]

Originally posted by mlinder I guess one drawback to programming this way is that if I break my very last "x" diameter tool, I have to go back to MasterCAM and recreate the code for a different tool.

Mark--

I program to the centerline of the tool instead of using the tool diameter. That way the toolpath is the same no matter what size of cutter you are using. Then in the control's cutter comp just use the actual size of the cutter as the offset. If you break your last 5/8 end mill jsut throw in a 1/2", change the offset and go!

You must watch out for lead in/lead out values if you are going to use a larger tool than originally planned for and stuff like that but under normal circumstances there is rarely a problem.