[popspipes]

I make several profile parts with the same cutter, when I sharpen the cutter I go into cam and change the diameter, this works.

What I was wondering is if I sharpen the cutter can I use cutter comp in Pathpilot for the new diameter? I watched a Saunders video on cutter comp, come to find out as near as I can tell that it uses the diameter in the tool table?? For some reason I never knew this, just ignorance on my part I guess. I had it in my mind that it had to be turned on or a g code entered to use it, this is evidently not the case??
I have 8 or more programs that use this cutter and its a pain to change the diameter in all those programs when it can be changed in Pathpilot from what I have seen once and done......

Any insight on this is very welcome...............

[machinehop5]

...would depend how the cutter path is written in each program. the Leadin and Leadout rules would have to be followed.
https://tormach.com/cutter-compensation-g40-g41-g42

a Negative offset value would work to comp for the Undersize amount from the Programmed cutter Diameter.
example like...programmed for EM1/2"(.500) and using a .460 EM the offset would be -.040

[popspipes]

I just watched this video again and John is changing the diameter of the tool in the PP tool table only.

What I want to do is to make the sharpened tool cut the same size as the original.

Can changing the diameter of the tool in PP's tool table accomplish this?

[mountaindew]

I just watched this video again and John is changing the diameter of the tool in the PP tool table only.

What I want to do is to make the sharpened tool cut the same size as the original.

Can changing the diameter of the tool in PP's tool table accomplish this?

I don't do production and never set up cam programs this way!
Not to say there is not a way to change this behavior and allow for compensation in cam programs. As mentioned before this would need to be setup in the cam program also.
I can't imagine having 5-25 cnc mills running the same program with different size cutters and not setting up the program to use the diameter of tool also!

The way I have sprutcam setup the code generated could care less what value is stored in the tool table diameter field at path pilot control. The sprutcam code only uses the height value stored in Path pilot at machine.
The 24r router with e.t.s. does not even use the height and only uses the tool description field stored on path pilot to display on screen. All other settings are cam and height is set with ets before each op.

[popspipes]

MD, this is the way I have been doing it in Sprutcam. It is just a real pain to change all the programs each time the cutter is sharpened and I was looking for an easier way.

The cutters are cheap enough that I can just use a new one when they get dull, I only cut aluminum so nothing exotic is really needed.

I dont run production either, may be 3 to 4 days then nothing for a few days, mainly hobby type stuff.

Machineshop5, thanks for your input on this as well I knew about the cutter comp g40 41 42, just never used it, this would have to be added to the programs each time I ran those parts, just looking for a simpler way.


this is the video in question, he was using it to increase the size of hole machined holes, I just thought it may work in my situation.

https://www.youtube.com/watch?v=Mxtf...channel=NYCCNC

[vmax549]

To use cutter comp the program HAS to be programed to use G41/42 and G40. Once the program is programed correctly then all you have to do is change the value in the tool table to match your tool . There are several ways you can apply the comp but that is your choice.

Now wether your cam can program cutter comp correctly is a different subject.

(;-) TP

[popspipes]

To use cutter comp the program HAS to be programed to use G41/42 and G40. Once the program is programed correctly then all you have to do is change the value in the tool table to match your tool . There are several ways you can apply the comp but that is your choice.

Now wether your cam can program cutter comp correctly is a different subject.

(;-) TP

I will experiment with it, I just have never needed it on the simple parts I make.

[TurboStep]

Hi Mike,
I never used it in Sprut and I've only tried it once in Fusion but you would only need to change the setting in Sprut highlighted in orange on the NYC screenshot. It probably only makes sense for finishing passes like contours. The diameter set in Sprut is then only used for the simulation and the diameter set in PathPilot is used for the actual milling. The lead in must be "at least as long as the tool radius" but Sprut should take care of this and the G41/G42 selection for you. Once you've simulated in Sprut and generated the code you would only need to make fine adjustments to the diameter in PP. The g-code remains unchanged.
Disclaimer: While I've only tried this once I never actually used it to machine a part because I didn't like the lead in created by Fusion for my specific application.
Take care
Step

[popspipes]

[QUOTE=TurboStep;2419008]Hi Mike,
I never used it in Sprut and I've only tried it once in Fusion but you would only need to change the setting in Sprut highlighted in orange on the NYC screenshot. It probably only makes sense for finishing passes like contours. The diameter set in Sprut is then only used for the simulation and the diameter set in PathPilot is used for the actual milling. The lead in must be "at least as long as the tool radius" but Sprut should take care of this and the G41/G42 selection for you. Once you've simulated in Sprut and generated the code you would only need to make fine adjustments to the diameter in PP. The g-code remains unchanged.
Disclaimer: While I've only tried this once I never actually used it to machine a part because I didn't like the lead in created by Fusion for my specific application.
Take care
Step[/QUOTE


Good to hear from you Step!
I use the tool table in Sprutcam for tool diameters, Pathpilot tool table for tool lengths, I didnt know that the diameter in the Pathpilot tool table was used for a program written in CAM or that it had any bearing on it?? Lots of things I dont know ha! When I get some time I am going to experiment with it. It would make my life simpler if that was the case just to change the diameter in PP at the machine for a reground cutter.


]

[mountaindew]

To use cutter comp the program HAS to be programed to use G41/42 and G40. Once the program is programed correctly then all you have to do is change the value in the tool table to match your tool . There are several ways you can apply the comp but that is your choice.

Now wether your cam can program cutter comp correctly is a different subject.

(;-) TP

I always figured if I did cam setups for others it would require this. That way all aspects of the program can be tweaked at the control.
My Cam software will do it. More dependent on the pp post and the g code it generates.

[popspipes]

I took a quick pic of my startup line in PP and there is a g 40 already in it, so John Saunders may be correct in his video as the function is already turned on. I just need to try it and see what happens, if this works it will save me some headache and time as I do sharpen and size cutters on occasion, (counterbores etc).

I posted the wrong pic, deleted it, but it still shows in the thumbnail sorry about that.

[TurboStep]

Hi Mike
G40 means "G40 - turn cutter compensation off.". I don't watch John's videos - I don't think he's the best reference. The functionality is available in PP but many special features won't work if cutter compensation is active so the initialization makes sure it's off.
To use it the program has to either set G41 or G42 depending on which side of the part outline the tool should follow (like climb or conventional). Sprut should handle this and hopefully also return to G40 afterwards.
Step

[popspipes]

Hi Mike
G40 means "G40 - turn cutter compensation off.". I don't watch John's videos - I don't think he's the best reference. The functionality is available in PP but many special features won't work if cutter compensation is active so the initialization makes sure it's off.
To use it the program has to either set G41 or G42 depending on which side of the part outline the tool should follow (like climb or conventional). Sprut should handle this and hopefully also return to G40 afterwards.
Step

Learned something new again!

[popspipes]

From what I am seeing so far, this isnt a simple solution for what I am trying to do!

[popspipes]

duplicate post..

[popspipes]

John set cutter comp in fusion before changing values in PP tool table. After about the fourth time watching the video and setting it HD I could see that it was turned on.

There is cutter comp in sprutcam.

I use stock to leave to produce the same results.

Thanks for all the input!

I need to not use sharpened cutters for the 4 versions of this part.

[vmax549]

It can be as simple as your programing skill or CAM allows it to be (;-) Try it you MAY like it . It is the easiest method to sneak up on a tolerance.

(;-) TP

[toyshop]

In fusion you can specify if the cutter comp is in the program or in the machine controller.. Unfortunately every time I tried checking in the machine I ended up with problems.
I haven't used it enough to figure it out if it was me or communication with PP. and now it's been a few months since I used a fusion program and just discovered the rapid limitation. A five inch long profiled part was almost 40 minutes.
Should have been about 10.

At my skill level I don't mind a separate program for each tool but the the slow rapids suck.

Dave

[soofle616]

I had a lot of issues with cutter comp when I first got into this stuff. Eventually I landed on using it as a wear compensation rather than a true diameter. There's a whole long story behind that and I'll probably confuse the issue trying to recount it. Short version, in Fusion (not sure if sprut has this option) I turn on cutter comp with "wear" selected. This causes fusion to output the g41/g42 codes as needed but the generate toolpath will still be calculated based on the tool diameter in the fusion tool library (nominal cutter size). Then in the machine tool table I enter a value to indicate the tool's variance from nominal. So if a 1/4" cutter is actually .249, I could enter -.001 as the tool diameter. If the tool is .251 I enter .001. The machine then adjusts the nominal diameter tool path to account for the change. In practice, the few times I've cared enough about a dimension to do this, I will pre-emptively enter a positive value to make the machine think the cutter is too big by a couple thou. Then I can bring that down a little bit at a time and rerun the cut to walk in to the final dimension. This approach has been much more successful for me than trying to enter the actual tool diameter. That always led to lead in length errors when I loaded the program into the machine. YMMV

[machinehop5]

x2 ..soofle616

..its up to the programmer vs program. CAD is the part contour path. CAM is how its machined.