View Full Version : Article on Cutter Radius Compensation, Summer 2011 Digital Machinist
06-17-2012, 01:44 AM
First, understand that I am not doing digital machining at this time, but I am trying to read as much about it as possible in preparation for the time when. Now, I have read and re-read this article several times and there is one thing I do not understand. I hope someone here can provide an insight.
The authors talk about using the cutter compensation commands, G41 and G42 to make adjustments for different sized cutters, mostly to account for reductions in their size after resharpening. OK, I can understand that and it sounds like a good idea in a production situation. But they talk about a problem the can pop up at the beginning of the cut when using that compensation. Apparently as the cutter approaches the work piece, there can be some kind of delay in coming to the final cutting line and this can leave a small, wedge shaped protrusion at a corner or something similar at another starting point. They then proceed to explain how to handle this problem. What they do not explain is why this problem occurs or if it is limited to only the software he is using or is it a more general problem. At least one of the authors are with Tormach so it may be limited to their software.
Can anybody explain why this happens and how general it is?
06-17-2012, 06:32 AM
Almost never happens since most cam software does cutter comp in post, not on the machine. You can tell it to let the machine handle it but I think most people don't.
06-17-2012, 09:43 AM
Never heard of that sort of problem unless manually programming some glitch in your program. Have seen some oddities in a few posters, but nothing serious.
Is the article on the net somewhere to read?
06-17-2012, 03:28 PM
I don't know if the article is anywere on the net, it was published in the Summer, 2011 edition of Digital Machinist as I said. Perhaps they put it on the Tormach web site: I will look.
Beginning to sound like a Tormach problem. Perhaps that article should have been designated as an advertisement.
I am curious because at some point in the next year or two I will be selecting some software to use in my first attempt at CNC in my shop. I am not sure what machine I will run it on yet, but I am determined to jump in soon.
06-17-2012, 05:09 PM
Main differences between getting the CAM to do it and the machine is that in CAM any deviation on size requires it to be reposted after editing the tool diameter.
On the Machine you can quickly change the tool diameter in the tool table on the machine.
CAM is for ease of working.
Machine is usually long production runs where you have to tweak sizes.
In CAM run in's and runs outs are not necessary, you can plunge down.
On the Machine they are necessary and have to be at least 1/2 the tool diameter in length, often more, depends on the controller to allow the offset to work.
09-07-2012, 09:06 PM
I think you are refering to approaching a side of the part straight on, in the middle of the side ( for example) and then turning ( rt angle) to follow the part with your cutter compensation . This would leave a wedge equal to the radius of the cutter.
If instead, You approached the same line (matching the side), but off the part, the cutter would now move with full cutter compensation and then run into the part, without leaving a wedge on the side.
In simple terms, Cutter comp is never actuated on the first move, it will only engage on the second move ( after a g41/42), and if the start of the second move is not on the part, no extranious edges are left
03-15-2013, 08:51 PM
When programming a CNC mill I have always used cutter comp. Several reasons. The program is cutter independent. The tool path is the actual size of the part without the compensation, easier to program. I don't have a sharp 1/2" endmill, I'll just use a 3/8". I often rough and finish, even for a quick one off. Tell it that the tool is larger and leave 5 to 10 thousands all around. Measure the part, change the tool comp, run again and the finish size is dead on.
I always apply tool comp BEFORE lowering the Z axis. I like to move to a position near the start about equal to the tool diameter away, call tool comp, make a short move of about 10 thousands towards the part. The tool moves over during that move, and you can lower the Z to the cutting depth clear of the part, or into a slot or pocket. Next move is on to the part. I like to use an arc, so it doesn't leave a mark from a sudden change in direction and a little overshoot. I also like to arc off the part at the end, starting at the same place I started.
I nearly always put all the moves in a subroutine. I use variables to pass the Z depth and the cutter comp. Set your variables, call the sub, change your Z, call the sub. You've reached the bottom change the comp variable, call the sub for a finish pass.
I like to use a variable for what I call Z Safe too. Z Safe is my retract height before a rapid. I initially set Z Safe to a height that I am SURE will clear all the fixtures clamps etc. Once I run the program, in the air or cutting, and I see how much clearance I really have I just change Z Safe to keep the tool down close to the work if I can.
Hope this helps,
Gary H. Lucas
03-16-2013, 08:51 AM
If you are using G41, G42, you do indeed need to give the machine time to know which side of the line it is on.
What I generally do is to start cutting in mid air, in the general direction of the first desired cut.
Sometimes I do make mistakes; on my blog, the Worden Cutter Grinder radius jig nut does have a little blip on it, as mentioned in the blog. (http://cnc-for-model-engineers.blogspot.com)
My mistake; should have fixed it, but it's probably better to show mistakes so others can see that I'm far from perfect!
I'm learning GCODE, because eventually I want to write my own pseudo-CAM routines, so I don't mind experimenting.