What's new
What's new

To compensate or not to compensate, that is the question. (Tool Dia compensation)

How do you compensate your tool diameter?

  • Put the diameter into the machine offests.

    Votes: 6 18.8%
  • Put only tool wear into the machine offsets.

    Votes: 22 68.8%
  • A mixture of both.

    Votes: 2 6.3%
  • Neither

    Votes: 2 6.3%

  • Total voters
    32

BluishInventor

Aluminum
Joined
Jul 7, 2020
I was curious as to how your shop operates with regards to programming at center path or with diameter comp. Do you comp diameter at the machine or do you only comp for wear?
 
Twenty-ish years ago when I was new and there was no cam system in the shop, and if there was only an odd size endmill sharp in the place, I would program on the line and use the comp and let the machine do the math. Since then the only comp I use now is for wear.

It was good when you had to figure stuff out with a calculator and scrap paper but not anymore.
 
If the size of the tool needs to be drastically changed, then most likely the program needs an edit (speeds feeds leads etc) Wear comp only.
 
Sometimes it is nice to program to the part print numbers and use the comp.
Bob


OK, so I'll be the asshole again and ask: When is it NOT nice to program the print numbers?
Can someone PLEASE give me an answer when is it preferable to have wear, and WHY!!!:scratchchin::scratchchin::scratchchin::toetap:
 
OK, so I'll be the asshole again and ask: When is it NOT nice to program the print numbers?
Can someone PLEASE give me an answer when is it preferable to have wear, and WHY!!!:scratchchin::scratchchin::scratchchin::toetap:

Biggest reason is leads. Lots more, like the one I mentioned above.
Also, most program in CAM so there really isn't a need to simplify the code for manual editing. Post and go. No need to sit and read code at the machine trying to picture where a pocket op is cutting. If I'm going to fingercam something, ya, I'll prob use Diameter but not sure why I would want to fingercam anything.
 
If you're finger camming for your '93 Fadal, sure, use diameter. If you want to do things the modern way, you let the software do the work, and you're not going to be man-reading that dynamic roughing anyway. Also, keep the appropriate cutters in stock; if you run out of 1/2" endmills you've got bigger problems. And unless you're a hobbyist, once you figure the lost labor and productivity, regrinds are more expensive than new, so there goes that excuse.
 
I think that the world of leadins and outs and the confusing or frustrating errors sometimes encountered are one reason many hate using full tool comps.
That move is sort of weird as the comp comes on depending on where you are to the tangent point of the first line or arc.

Wear comps and tool dia. comps are the same thing to a control and are just added together.
Difference is small move vs big move. The small move is much more tolerant to the point of not a worry 99.9999% of the time.
Put 0.5000 into the wear comp and back to the old problem. :)

With newer controls or CAM is also the feedrate at tool OD vs tool center-line when doing arcs or circles. Some stuff wants to know actual tool dia to correct and some ignores it.
If you lie to the machine about tool size no matter how good or smart the fancy control it can not help you.
Bob
 
I think that the world of leadins and outs and the confusing or frustrating errors sometimes encountered are one reason many hate using full tool comps.
That move is sort of weird as the comp comes on depending on where you are to the tangent point of the first line or arc.

Agreed, it is what confuses people, but there is nothing weird about the lead-ins/outs.
Nothing!

As far as Finger vs AnyCAM, Who Cares!!
Be consistent and write the program the same way all the time!!!
I'm about 10% finger 90% CAM, but at the end of the day all programs are Full, never a single program that is not!

Resharps? I don't own a single one that I use for production.
 
With newer controls or CAM is also the feedrate at tool OD vs tool center-line when doing arcs or circles. Some stuff wants to know actual tool dia to correct and some ignores it.
If you lie to the machine about tool size no matter how good or smart the fancy control it can not help you.
Bob

Exactly!
So you want CAM to figure out the compensation, and yet you want the machine do the SFM/IPR calculations?
To achieve that, you put in 0 for tool dia and something for wear.
But now you have to tell the machine what size the tool actually is in order for it to calculate the RPM and IPM based on your programmed SFM/IPR.
To achieve that, you now have to enter the actual diameter into the control somewhere else ..... :nutter:

Why not just put in the actual dia in the offset page, put in the small deviation ( plus or minus ) into the wear offset and let the machine have at it?
 
Why not just put in the actual dia in the offset page, put in the small deviation ( plus or minus ) into the wear offset and let the machine have at it?
I guess we each have our own private little crusades :) Mine is the metric system, at least yours has a chance of winning ...

(Always been a CL fan myself, even for manual programming, don't like long lead-on lead-off moves but oh well.)
 
Exactly!
So you want CAM to figure out the compensation, and yet you want the machine do the SFM/IPR calculations?
To achieve that, you put in 0 for tool dia and something for wear.
But now you have to tell the machine what size the tool actually is in order for it to calculate the RPM and IPM based on your programmed SFM/IPR.
To achieve that, you now have to enter the actual diameter into the control somewhere else ..... :nutter:

Why not just put in the actual dia in the offset page, put in the small deviation ( plus or minus ) into the wear offset and let the machine have at it?

The only time you'll get compensated feedrates is when using full diam comp. So your roughing passes will not have this adjusted feedrate, unless you are comping all those too, which would be ridiculous....so not much of an argument here. Besides, this can be controlled in CAM as well.

I think the divide here is the old way of relying on the control vs the new way of relying on CAM. Most at this point have switched to using and relying on CAM.
 
.... So your roughing passes will not have this adjusted feedrate, unless you are comping all those too, which would be ridiculous.....
Clueless on ridiculous here. Unsure why roughing not the same.:confused:

Life was so much simpler in the days of paper tape and none of this confusing correction and compensation computer stuff. :)
Back then no edits unless you liked to splice tape or punch a whole new one. Done right or fail.
Bob
 
Clueless on ridiculous here. Unsure why roughing not the same.:confused:

Life was so much simpler in the days of paper tape and none of this confusing correction and compensation computer stuff. :)
Bob

You will have look ahead issues and even problems with rads smaller than your cutter, cutter path crossing itself...forgetting to turn off on when retracting...the list goes on and on.

The paper tape days, the problem with not having comp or cam was all the trig that had to be done lol
 
I think the divide here is the old way of relying on the control vs the new way of relying on CAM. Most at this point have switched to using and relying on CAM.

So why even bother to switch to relying on CAM?
Your programs will be different, and yet, the actual cutter movements will be absolutely identical.
I mean if CAM doesn't care, machine doesn't care, but your program is readable ( whether you want to even look at it or not ) ... what's the harm?


Sidenote: Wonder who is the 1 person using NEITHER!!!
 
Sidenote: Wonder who is the 1 person using NEITHER!!!

I know of a "programmer" who does exactly that. Program centerline and no comp. After measuring the first part, he goes back to Fusion to adjust stock to leave, then re-posts the program.

Also know of a different guy who wouldn't adjust countersink tool length offsets at the machine (because it will mess up other programs!) and instead adjust the CAM program to get the right dia...

Both guys been doing this several years. Maybe 10 or more.

Sure are crazy people out there.
 








 
Back
Top