G41/G42 CUTTER COMPENSATION

This forum is for general discussion about Aspire
User avatar
Leo
Vectric Wizard
Posts: 4083
Joined: Sat Jul 14, 2007 3:02 am
Model of CNC Machine: 1300 x 1300 x 254 Chinese Made
Location: East Freetown, Ma.
Contact:

Re: G41/G42 CUTTER COMPENSATION

Post by Leo »

FixitMike wrote:I'm confused. Isn't cutter comp G41/G42 part of the G code file? Or used with the machine controller? Why not add it to the G code file with a text editor?

If you want Aspire to modify the toolpath, you have to open the Aspire program, modify as desired, recalculate and save the toolpath, and resend it to your CNC. Regardless of whether the modification is to a hypothetical cutter comp, offset, or tool diameter. I don't understand why it is desirable to have it done in Aspire if the objective is to correct for the actual tool diameter.

On further thought, I do see where it would be advantageous if you are using the "Output direct to machine" feature. But otherwise, no. And I would be concerned about what happens the next time I used the toolpath. One more thing to check before pressing the Start button.
Mike, In aspire of other vectric products it would be located in the box to be Left - Right - On. There would be a box to use cutter comp. It would also be dependent on climb or conventional.

If someone never used cutter comp before I suppose it would be difficult to realize the benefits of having it available. BUT - if someone used it extensively in the past, they would not understand why it's not part of the package. Personally, I wish it was part of the package - I would use it all of the time on pocketing and profiling.
Imagine the Possibilities of a Creative mind, combined with the functionality of CNC

LittleGreyMan
Vectric Wizard
Posts: 1012
Joined: Fri May 15, 2015 1:10 pm
Model of CNC Machine: 3 axis small size machine
Location: France

Re: G41/G42 CUTTER COMPENSATION

Post by LittleGreyMan »

Leo,

It's probably obvious for you and all people that already used that on industrial CNC, but not for mere mortals. That's why we have some difficulties to understand.

I think I know the general principle, but correct me if this explanation is wrong.

When you use the cutter compensation, the CAM software calculates the toolpath as usual. But when you run the code on the CNC, the controller asks you the compensation (difference between the actual diameter tool and the theorical one) and handles the difference.
Best regards

Didier

W7 - Aspire 8.517

ger21
Vectric Wizard
Posts: 1592
Joined: Sun Sep 16, 2007 2:59 pm
Model of CNC Machine: Custom DIY
Location: Lake St Clair, MI, USA
Contact:

Re: G41/G42 CUTTER COMPENSATION

Post by ger21 »

There are a couple different ways to use G41/G42.

One way, as you say, is to program with a certain size tool, with the CAM offsetting the toolpath, and then the control adjusts the toolpath for the actual tool diameter.

The way I use it, which is common with industrial routers ($100K and up) is to program on the line, and let the control offset the toolpath the radius of the tool.
Gerry - http://www.thecncwoodworker.com

LittleGreyMan
Vectric Wizard
Posts: 1012
Joined: Fri May 15, 2015 1:10 pm
Model of CNC Machine: 3 axis small size machine
Location: France

Re: G41/G42 CUTTER COMPENSATION

Post by LittleGreyMan »

Thanks for clarifying Gerry.
Best regards

Didier

W7 - Aspire 8.517

User avatar
Leo
Vectric Wizard
Posts: 4083
Joined: Sat Jul 14, 2007 3:02 am
Model of CNC Machine: 1300 x 1300 x 254 Chinese Made
Location: East Freetown, Ma.
Contact:

Re: G41/G42 CUTTER COMPENSATION

Post by Leo »

There is a tool offset register in the machine. Generally, on industrial machines, there is a length geometry and a Diameter geometry offset. The M06 G43 Txxxx line picks up the offsets.

In the G-Code program, either method can be used as Ger21 noted. IF ON the line is selected - then the actual tool radius would be entered into the offset register in the machine. Most machines also have a "wear" offset for the same tool. That is where adjustments are made. IF - the right or left were programmed in the G-Code - then "0" would be entered in the tool radius offset in the machine.

With either option, the end result is the same.

NOW - HOW it is used is like this.

Suppose you were making a 1" hole and you wanted to fit a 1" dowel into the hole. NICE fit - really NICE fit. You are using a 1/4" end mill. So you circular interpolate the hole. Fancy words for pocketing the hole.

When you try the dowel and it does not fit - BAM - you pound your fist down. NO - not with cutter comp you don't. What you do is go to the "WEAR" offset for that cutter and adjust it a couple of thou and rerun the hole. Takes 10-15 seconds. BOOM - tweak the hole up until that dowel fits perfect. SWEET

I guarentee that it will take some learning to get the understanding down - but there is nothing better.

Going into Vectric and changing the cutter diameter is basically the same thing, but you then need to recalculate, repost, reload into the machine, then rerun. That is a whole lot more cumbersome. Like I said Cutter Comp is 10 - 15 seconds - TOPS -- really not even that long.
Imagine the Possibilities of a Creative mind, combined with the functionality of CNC

User avatar
Leo
Vectric Wizard
Posts: 4083
Joined: Sat Jul 14, 2007 3:02 am
Model of CNC Machine: 1300 x 1300 x 254 Chinese Made
Location: East Freetown, Ma.
Contact:

Re: G41/G42 CUTTER COMPENSATION

Post by Leo »

SORRY

I posted that a little wrong

The G43 picks up the length off set not the radius offset.

The G41/G42 is what picks up the radius offset.

G40 cancels the cutter comp offset
Imagine the Possibilities of a Creative mind, combined with the functionality of CNC

LittleGreyMan
Vectric Wizard
Posts: 1012
Joined: Fri May 15, 2015 1:10 pm
Model of CNC Machine: 3 axis small size machine
Location: France

Re: G41/G42 CUTTER COMPENSATION

Post by LittleGreyMan »

Thanks for your comments Leo.

I'll add it also allows using sharpened tools which diameter has slightly changed without entering each one in the database. You use a 10mm tool in the CAM software and use cutter compensation in the shop when you choose the 9.94 mm sharpened tool. Much easier and avoids mistakes.
Best regards

Didier

W7 - Aspire 8.517

ger21
Vectric Wizard
Posts: 1592
Joined: Sun Sep 16, 2007 2:59 pm
Model of CNC Machine: Custom DIY
Location: Lake St Clair, MI, USA
Contact:

Re: G41/G42 CUTTER COMPENSATION

Post by ger21 »

LittleGreyMan wrote:Thanks for your comments Leo.

I'll add it also allows using sharpened tools which diameter has slightly changed without entering each one in the database. You use a 10mm tool in the CAM software and use cutter compensation in the shop when you choose the 9.94 mm sharpened tool. Much easier and avoids mistakes.
Yes, this is how and why I use it. We cut cabinet parts every day, and 90% of the time, the tools in the machine have been sharpened to various sizes. Only about 10% of the time do we use the 1/2" bit we programmed for. The rest of the time the bit's are between .420" and .485", and the G41/G42 adjusts automatically.
Gerry - http://www.thecncwoodworker.com

Post Reply