How Do You Apply Cutter Compensation ?

[jonbanquer]

Found this quote today while reading a manual from another CADCAM program. It applies to BobCADCAM and how people maybe taught or are using cutter compensation:

"WARNING: The system does a much better job offsetting the tool than the majority of controls currently available. Regardless of the setting made in the preference, all toolpath drawing and cut part rendering will be calculated and displayed using the system's offsetting mechanism. Therefore, it is possible for the cut part rendered image produced by the system to look good, while the tool cutting according to the posted code, will not cut well. If the control's offsetting mechanism is less advanced than the systems it is possible when the control produces the offset values, errors and interference will result."

In my opinion I don't believe anyone should be using a CNC control to figure out cutter compensation. BobCADCAM should be used to figure out cutter compensation *not* the control.

Anyone care to argue differently ?

jon

"I may have many faults, but being wrong ain't one of them." ... Jimmy Hoffa

[ger21]

Your quote says what if the controls comp is less advanced than the CAM's. What if it's more advanced?

On our router at work, I use G41/G42 99% of the time. Cutting wood, we get several sharpenings out of our bits, and the comp let's us use any bit we want, regardless of the size. If we need to replace a bit during a run of parts, just change the tool table, and keep on running with identical results. If I need to take a few .001's more off, just change the diameter in the tool table.

Prior to using comp all the time, we would get a lot of mis-sized parts due to not knowing the diameter of the tool in the machine. We may run hundreds of parts in a single shift, and don't have the luxury of knowing the exact size tool we'll be using when we run the parts. Cutter comp makes this a non-issue.

I'm sure most software vendors will tell you that their software works better than something else. If you use the controls comp, you'll find out very quickly if it works or not. If it works, I say use it.

[jonbanquer]

"What if it's more advanced?"

Even it it was I would rather the CADCAM system did the cutter compensation. If there is a problem I know for sure where the problem is coming from.

Based on my experience with machines like FADAL's I tend to doubt anything FADAL has in their control software would be more advanced.

Why chance it ?

jon

"I may have many faults, but being wrong ain't one of them." ... Jimmy Hoffa

[HuFlungDung]

I'd agree with Ger. It's a lot handier to tweak the tool comp register in a mill than run back and forth reposting the program in cadcam. But, you must have a good controller that is capable and trustworthy.

Still, I tend to reserve tool radius comped paths for those situations where final dimension is really critical, otherwise I do usually just let the CAM do the compensated path.

For lathe paths, I usually let CAM do the compensated path, because the insert radius is some well known nominal dimension, and it would be very unlikely that I would tweak the toolnose radius even once for a lathe toolpath. Any discrepancy from final dimension would be taken care of with X or Z offsets. Of course, I'm not talking about high precision demands that would require an optical comparator to see if the generated radius really is exactly correct.

[jonbanquer]

"I'd agree with Ger. It's a lot handier to tweak the tool comp register in a mill than run back and forth reposting the program in cadcam."

I never do this. If it's a critical tolerance I enter positive D comp... say .003 and go from there. What I don't do is enter half the radius of the tool and let the CNC machine do the cutter compensation.

jon

"I may have many faults, but being wrong ain't one of them." ... Jimmy Hoffa

[tjones]

Both right? In 2D I let the machine comp, in 3D I let the CAM comp. In 2.5D I let CAM comp.

[HuFlungDung]

I'd argue that if there are G41's or G42's in the code, then you are using machine comp. Whether its full tool radius or only the wear amount, its still the control compensating for the radius of the tool.

I can see the argument for 'safety' in using small values in the comp register, so long as everyone in the same shop has the same understanding about how comp is used throughout that entire organization. That is the real danger, is the potential harm arising from a simple misunderstanding between programmers and machinists, about what is considered standard practise.

[Geof]

If it's a critical tolerance I enter positive D comp... say .003 and go from there. What I don't do is enter half the radius of the tool and let the CNC machine do the cutter compensation

This does not make any sense. If you are entering any value into the tool compensation table you have to then have G41 or G42 in your program to use this value so the machine controller is doing compensation.

[jonbanquer]

Originally Posted by HuFlungDung I'd argue that if there are G41's or G42's in the code, then you are using machine comp. Whether its full tool radius or only the wear amount, its still the control compensating for the radius of the tool. I can see the argument for 'safety' in using small values in the comp register, so long as everyone in the same shop has the same understanding about how comp is used throughout that entire organization. That is the real danger, is the potential harm arising from a simple misunderstanding between programmers and machinists, about what is considered standard practise.

I agree it's still a form of cutter compensation but the small offset is much easier on the control.

As you correctly point out safety is an issue when the full radius of the tool has to be entered all the time !!!

I have not worked in a machining job shop in over 10 years that enters the full tool radius amount in the CNC control ! I would argue that having the CADCAM system do cutter compensation is considered standard practice in Phoenix, Arizona.

I think the reason BobCADCAM is taught not fully offsetting the profile is that in BobCADCAM it takes *longer* to offset the profile. (Unless your using V20's new Profile wizard). Other CADCAM systems of course do this automatically and have done so for years. In my opinion, the video tutorials should show offsetting the profile as this is safer and pretty much the norm as far as I'm concerned.... just another reason to sell videos and not require a user to attend a seminar.... can you imagine the arguments over this one ?



jon

"I may have many faults, but being wrong ain't one of them." ... Jimmy Hoffa

[jonbanquer]

Originally Posted by tjones Both right? In 2D I let the machine comp, in 3D I let the CAM comp. In 2.5D I let CAM comp.

Most of the time you don't have a choice when doing surfacing toolpath unless you have a very sophisticated control. I have heard that Fida is such a control.

jon

"I may have many faults, but being wrong ain't one of them." ... Jimmy Hoffa

[YNKEY]

In The Beginning Before Cad Cam We Had To Manually Program And Punch In The Code It Was Much Easier To Program The Actual Line And Then Use Cutter Comp To Rough, Finish Cham Or Whatever Using The Same Program As Long As Your Cutter Was Smaller Than The Smallest Radius. Never Had Any Trouble With The Control Not Figuring It Right. Lie .002 To The Cutter Check And Adjust