Page 1 of 1
Cutter Comp Wear Only?
Posted: Mon May 17, 2021 12:43 pm
by ridekp
Hi All,
No problems with my machine for this post, just a general question about CNC 12. I would like to use cutter comp with wear only, letting my CAM software program to the theoretical tool diameter. I was thinking this would be very simple but I found out today that CNC 12 will not let you put a negative number in the diameter box. On other industrial controls there are separate columns for diameter and wear but I don't think this is really necessary as long as your can enter positive and negative values for your compensation.
I know the answer is to tell my CAM to use the tool diameter in my control which would allow me to compensate either positive or negative to that starting point. However I dislike doing this for a few reasons. My machine is in imperial units and I use a fair amount of metric tooling. This makes it very hard to see which tools I have applied compensation to since I don't have metric conversions memorized down to the tenths. I also don't have a way to probe the diameter of my tool so I'd just be starting at the theoretical dimension of the endmill anyway. I prefer to just see the amount I have compensated the endmill since most of my usage is dialing in a fit, not necessarily compensating my tool to be the actual diameter it is. It may just be my preference, but I also dislike seeing my CAM toolpaths on the line rather than offset where the tool will actually be.
If I am missing an easy way to just use wear comp, please let me know and disregard the past two paragraphs. Otherwise, is there a way to make CNC 12 accept negative numbers in the tool diameter box? If there isn't, is this an easy addition that can be added to future versions of CNC 12?
Thanks for reading!
Re: Cutter Comp Wear Only?
Posted: Mon May 17, 2021 2:58 pm
by swissi
ridekp wrote: ↑Mon May 17, 2021 12:43 pm
Hi All,
No problems with my machine for this post, just a general question about CNC 12. I would like to use cutter comp with wear only, letting my CAM software program to the theoretical tool diameter. I was thinking this would be very simple but I found out today that CNC 12 will not let you put a negative number in the diameter box. On other industrial controls there are separate columns for diameter and wear but I don't think this is really necessary as long as your can enter positive and negative values for your compensation.
I know the answer is to tell my CAM to use the tool diameter in my control which would allow me to compensate either positive or negative to that starting point. However I dislike doing this for a few reasons. My machine is in imperial units and I use a fair amount of metric tooling. This makes it very hard to see which tools I have applied compensation to since I don't have metric conversions memorized down to the tenths. I also don't have a way to probe the diameter of my tool so I'd just be starting at the theoretical dimension of the endmill anyway. I prefer to just see the amount I have compensated the endmill since most of my usage is dialing in a fit, not necessarily compensating my tool to be the actual diameter it is. It may just be my preference, but I also dislike seeing my CAM toolpaths on the line rather than offset where the tool will actually be.
If I am missing an easy way to just use wear comp, please let me know and disregard the past two paragraphs. Otherwise, is there a way to make CNC 12 accept negative numbers in the tool diameter box? If there isn't, is this an easy addition that can be added to future versions of CNC 12?
Thanks for reading!
AFAIK, CNC12 can only do cutter compensation by adjusting the tool reference diameter up or down. I can see the problem you describe to identify changed tool diameters but I can offer you a solution for that when you use the Tool Manager of the ProbeApp.
The Tool Manager of the ProbeApp does read the tool information provided by the Post Processor at the beginning of a job file. Here's an example
Code: Select all
%
O01002
(1002)
(T1 D=4. TAPER=90deg - ZMIN=-1. - spot drill - 4mm Spot Drill)
(T2 D=10. CR=0.33 - ZMIN=-12.5 - bullnose end mill - Test Tool)
(T3 D=8. ZMIN=-12.5 - flat end mill - 8mm Flat Endmill)
(T6 D=4. ZMIN=-6. - flat end mill - 4mm Flat Endmill)
(T9 D=6. TAPER=45deg - ZMIN=-1.3 - chamfer mill - 6mm Chamfer Mill 45 Degreel)
(T12 D=6.5 TAPER=118deg - ZMIN=-14.953 - drill - 6.5mm Drill 118 Degree)
The Tool Manager will highlight all tools that don't match the tool dimensions from the CAM Tool library like this:
This will at least show you when you have changed a tool diameter in the CNC12 Tool Library and you can see the difference to the nominal size of the tool.
-swissi
Re: Cutter Comp Wear Only?
Posted: Tue May 18, 2021 12:03 pm
by ridekp
Thanks Swissi, that is a good way to check if they have been modified.
I'm kind of hoping Kieth can chime in with some insight as to whether this would be a simple edit or a non trivial change to implement. Would there be any down side to allowing a negative value in the diameter box? Is the goal just to keep people from making an unintentional mistake? Maybe, instead of an error box stating that a negative value is not allowed, it could be a warning highlighting that you are entering a negative value?
Re: Cutter Comp Wear Only?
Posted: Tue May 18, 2021 3:23 pm
by tblough
I suspect that it is a non-trivial change given that the backplotter uses the tool table diameter to graph the cutter. Graphing might have a problem trying to draw a cutter with a negative diameter.
Re: Cutter Comp Wear Only?
Posted: Wed May 19, 2021 12:22 am
by cncsnw
I found out today that CNC 12 will not let you put a negative number in the diameter box.
If that is true, then it is a recent development, and a step backward. From versions of CNC7 released in the 1990's, at least through version 4.14 of CNC12, Centroid's software has allowed negative diameter offset values, for exactly the reason you are wanting to use them.
G41 with a negative diameter should behave exactly the same as G42 with the same diameter positive; and likewise G42 with a negative diameter should behave exactly the same as G41 with the equivalent positive diameter.
Did this get broken in some recent CNC12 release for Acorn?
Re: Cutter Comp Wear Only?
Posted: Thu May 20, 2021 6:57 am
by ridekp
So now I'm thinking I must be crazy! I just fired up the machine again and I can now enter negative diameter values. I was hoping to grab a screen shot of the error and it worked as I expected it to originally. I wasn't able to run the part again but maybe the first time I tried there was some combination of g41/42 being active that cause the error the first time. I will try to use this method this weekend and report back if I run into any issues.
Re: Cutter Comp Wear Only?
Posted: Thu May 20, 2021 10:14 am
by slodat
I haven't used cutter comp yet. Can you explain your process. Let's say a feature is 0.001 bigger than you want, how do you use comp to take that off on the next part?
Re: Cutter Comp Wear Only?
Posted: Thu May 20, 2021 2:02 pm
by cnc_smith
Replaying to ridekp first.
Negative tool diameter
In your post I did not see what version of CNC12 Acorn you are running or if you are in imperial (inches) or Metric? Please post a Report. I tested with Acorn V4.60 in inches and you are able to use a negative number. I put a small number in and as large as -.0500 and it graphed correctly.
Replaying to slodat now.
How to adjust the cutter to cut the correct drawing dimension.
With cutter comp turned on and you are making a cut round the outside of a part using a .500 inch diameter cutter. When you measure the part and the cut dimension is larger than the programmed dimension (Drawing dimension) this means the cutter is smaller than .500. The amount you decrease the cutter size is a diameter value. If the cutter cuts on both sides of the part you are measuring you would decrease the the size of the cutter by that amount so it would offset more for the smaller cutter. If the cutter only cut on one side of the part you would decrease the diameter of the cutter by 2 times the measured amount. For an OD cut if the measured dimension was smaller than the programmed dimension then you would increase the cutter size by that amount.
For an ID cut like a Circle or rectangle if the measure dimension is smaller then you would decrease the size of the cutter so it would cut larger. If the ID was larger then you would increase the size of the cut so it would cut smaller.
Re: Cutter Comp Wear Only?
Posted: Fri May 21, 2021 12:29 pm
by ridekp
cnc_smith wrote: ↑Thu May 20, 2021 2:02 pm
Replaying to ridekp first.
Negative tool diameter
In your post I did not see what version of CNC12 Acorn you are running or if you are in imperial (inches) or Metric? Please post a Report. I tested with Acorn V4.60 in inches and you are able to use a negative number. I put a small number in and as large as -.0500 and it graphed correctly.
I am running 4.64 and using imperial units. In my last post I discovered that I was incorrect in my statement that CNC12 would not allow negative diameter values. When I stumbled into that perceived error, it was at the end of the day and I shut the machine off and walked away. When I went back to try and replicate the error I was able to enter negative diameter values. I may have entered a number incorrectly and caused a syntax error or I might have had g41 or g42 and some combination of other g codes still active when I tried to enter the negative value causing an error.