Centroid Community CNC Support Forum

I am just learning to use cutter compensation. I have taken the approach of using WEAR in Fusion 360. I have set all my initial tool diameters to 0. What I find is that when running a toolpath with roughing and finishing passes the 2nd finishing pass isn't effective. For example I used a sharpie to mark the part after roughing and the mark is gone after the first finish pass. I remark the part and after the second finishing pass there is a "shadow" of the mark, meaning it removed material, but not much. After thinking about it, it seems that it would be better to separate the roughing toolpath THEN do a finishing pass...maybe this is common knowledge. Running the entire toolpath became a PITA yeah I could've "run from"
Questions;

• Does CNC12 allow In Control? I haven't seen any info on how to apply it
  is there a minimum lead in requirement to start comp? If I'm using 1/8 cutter is 1/2 dia too much?

WEAR means you program for the nominal tool diameter, and then the tool diameter offsets are the opposite of how much the part measures over or under after the finish pass.

Set your diameter offsets to zero. Run your program. Measure your part. If the feature was supposed to be 2.000" and you measure 2.0025", then set your diameter offset for that tool to -0.0025" and rerun your finish pass.

As your tool wears, it gets smaller and pushes off more, you keep increasing your wear offset to compensate until you change your tool and start over from 0.

Your lead-ins need to be longer than your offsets.

I'm not 100% clear on what diameters should be in the tool table. I'd guess that when "in Computer" is used that CAM drives the tool diameter and when wear is used the diameter offset from the table is used. The tool diameter in my table are set to 0. What happens with Intercon?

"in cnc control" means the G code will have a G41 and G42 in it.. look up these G codes in the operator manual there are examples of how they work. page 215 of mill manual.
these codes use the tool diameter set in the tool library, these codes should have a proper lead in move to work correction as well has a lead out before a repeat.
easiest to practice with Intercon. Mill training video shows how to use cutter comp properly with cnc12/intercon.

I'd guess that when "in Computer" is used that CAM drives the tool diameter and when wear is used the diameter offset from the table is used. The tool diameter in my table are set to 0. What happens with Intercon?

If you are using certain tool/offset numbers with programs that you wrote using offline CAD/CAM, with cutter compensation "in computer" plus G41/G42 for wear offsets, then as you note, you start with 0.0 for the tool diameter in the Centroid Tool Offset Library.

As a rule, you cannot conveniently use those same tool numbers in Intercon programs. Intercon's canned cycles (pockets, frames, thread milling, etc.) require that the full cutter diameter be entered in the offset library.

In this situation, you will need to set aside some blocks of tool numbers to use with your CAD/CAM-generated programs, and different blocks of tool numbers to use with your Intercon programs.

If you have an automatic tool changer, and some of those different tool numbers actually refer to the same tool, you can use the "Bin" field in the Tool Library to tell CNC12 that both "tools" are in the same tool-changer pocket.

<snip>
As a rule, you cannot conveniently use those same tool numbers in Intercon programs. Intercon's canned cycles (pockets, frames, thread milling, etc.) require that the full cutter diameter be entered in the offset library.

In this situation, you will need to set aside some blocks of tool numbers to use with your CAD/CAM-generated programs, and different blocks of tool numbers to use with your Intercon programs.

That clarifies the Intercon questions
Is there a way to store a text version of the tool table and import it in for Intercon? Or just start Intercon tools at 101 as you said.
Maybe this would be a feature request to specify a tool table file for intercon, or just type in the diameters...?

I use CAT40 holders and am switching tools out fairly regularly so it may be a problem to keep it all coordinated. It's not like I am running a production shop. For my usual one off jobs tool measurement is SOP.
I use Intercon for drilling that wouldn't affect my table. Most programs come from Fusion 360 and it has only been this week that I considered using cutter comp. I usually use "In Computer" I've been making some nested circles and it's nice to sneak up on dimensions to make things fit

I have my tool library tools for my CAM system starting at 11 leaving me tools 1-10 for ad-hoc Intercon tools.