Compensation issue

[Georgi Baltov]

I think I am bugging you guys way too much but what can I do. Does these things only happen to me or when other people get something wrong prefer to call?

Anyways, here's what I got today when running some dovetail drawer boxes. BTW find all the files that I think you might need. Let me know if I have missed something.

I wrote the program with 3/8" DC bit @ .315". The bit was used quite a bit so I changed it before we started cutting to a brand new one @ .375". As far as I know the machine should compensate. But it didn't. Right where the male joints are it reliefs with the 3/8" bit and now it cut bigger hence making a gap on the inside of the box when you put it together.

I experimented and tried it the other way around. I wrote the program with the 3/8" bit @ .375" and then changing to .315". The machine compensated just fine. The joints fit great. Of course whole problem took me 2 hours to figure out. Initially I blamed my operator for not putting the right compensation. Well, I owe him an apology now.

I always thought compensation goes both ways. If I am wrong please excuse my ignorance, otherwise let me know if there's more I can help with.

Thank you

[Daniel Vonderheide]

Georgi,

The code is the same in both files for the male dovetail routs. The issue is the actual tool size. Your male dovetails have a spacing on the outside of .372 so a .375 tool will remove .003 on the opposite edge when cutting. The second thing is the radii inside the male dovetails is only .125 so you should only be using a .25 tool. I'm betting the error is still there with the .315 but it is less pronounced. I would recommend changing your male dovetail tool to a .25 tool. Hope this helps.

[Georgi Baltov]

Daniel,

I got it. It's a "Special Case". The dovetail tool is the 1/4" DC set at .249" (T304) if new (as recommended by thermwood). The problem is the T303 which is 3/8" DC. The depth of the dovetails is set at .35 so if T303 is .375" it won't use it. But the code was written with T303 sitting at .315" so when it was changed to .375 because it was still in the code it used it and it made the full dado .025 bigger. That's why I got the gap.

At the same time I have the same problem on some other parts of the cabinet. My top on base cabinets is .6875 thick so 50% blind dado makes it .3438. The program was written when T303 was .315 and then changed to .375" when we ran it. It made a big gap but the cabinet makers were able to clamp and hide it.

There's no way that you or I can prevent that. May be by hard-coding each different cut with specific tool but even then I am sure there would be these special cases.

The best way is to start with one tool and finish with it even if you loose $30 dollars in resharpening.

Thanks for the help

[Daniel Vonderheide]

You should always update the tool in tool manager first before nesting. If you change the tool diameter in the tool manager before you open Control Nesting, control nesting will recognize the size change and choose tools accordingly. If the tool changes from .315 to .375, there may be operations that it cannot perform anymore, like the dados you mentioned. Making sure the tool manager is accurate before nesting is the best way to eliminate these errors.