What's new
What's new

Tool offset while using G41

M Code

Aluminum
Joined
Apr 4, 2021
Hi

If I use G41 the geometric tool offset value will be the radius of the tool, I saw some machines they use the diameter in the geometric tool offset while using G41 I want to understand how they use the diameter ? is this related to the machine or programming way?

Thanks
 
Hi

...is this related to the programming?

Thanks
Cutter Comp is going to heavily depend on how you setup your comp in CAM. CAM doesn't know what you're putting in your Geo comp on the machine but you need to tell the CAM whether you want to comp in Computer, Control, Wear or leave it off entirely. Safest method is to use Wear, skip the geometry tab on the control and adjust size with the Wear column on the machine to fine tune size. This way CAM takes care of the nominal tool diameter and any fine adjustment can be done on the control without typing in any tool diameters from the beginning, just adjusting "Wear" to fine tune part size.

I know this doesn't specifically answer your question, as every control is different but it is a safer, more reliable method, IMO.
 
what do you enter in your machine offset if you run G41 and the program follow actual path the diameter or radius?
I NEVER program from the tool diameter, only the tool center, and use wear comp. I also only use radius comp, shop rules even in my own. I have tried programming with full radius comp a little but after beating my head silly for an hour trying to get a Fadal to run good code that is said wasn't and finally reprogramming from tool center to get it to run the program I never tried it again.
 
Even if diameter is entered in the offset table (depending on a parameter), the machine internally divides it by 2, to find out the radius. Radius compensation uses radius only.
 
I NEVER program from the tool diameter, only the tool center, and use wear comp. I also only use radius comp, shop rules even in my own. I have tried programming with full radius comp a little but after beating my head silly for an hour trying to get a Fadal to run good code that is said wasn't and finally reprogramming from tool center to get it to run the program I never tried it again.

No diameter and using wear is the opposite of how I was trained on a mill at the first replace I worked, we never used wear on a mill and only used full diameter for cutter comp. It was also all programmed with fingercam. It was tricky starting out trying to figure out how much you had to adjust the tool size to bring in a feature.

Now that I have my own place and it’s almost all cam, I think I’m going to switch as it makes a lot of sense. Normally code is straight from the computer using tool center and typically falls within the block tolerance on the prints, when it doesn’t I’ve just fixed it in cam and reposted rather than messing with the tool table. I figured let me adjust the size of a single feature vs all the features (in cases where deflection was the issue not the tools actually cutting diameter.) With cam I would never make a large tool diameter change at the control anyway so letting the computer keep track of the tool diameter seems best.
 
what do you enter in your machine offset if you run G41 and the program follow actual path the diameter or radius?
Hello M Code,
In theory, a Zero Value would be registered, but because of tool run-out, tolerance of the diameter of the cutter and tool spring, its common to have some small value, either plus or minus, to adjust the size of the feature.

When using Centre Line of Cutter, plus TNRC (G41/G42) and when running a part program for the first time, or with a change to a new tool, it's common practice to add a small positive Tool Radius Comp value so as to not cut the part out of tolerance. In this case, the feature is measured and the small Tool Radius Comp value adjusted to cut the feature in tolerance.

The same Tool Radius Compensation interference errors exist with programming centre of tool and using small values in either Tool Radius/Diameter, or Tool Wear specifications. as exists when programming using the Work-piece coordinates and full radius tool Radius/Diameter specified.

Lets say that a Concave Radius Feature has a radius close to that or the cutter being used. Its common and prudent to use the biggest cutter that the geometry of the part will permit (to minimize push off of the tool). So, in this example part, there is a concave feature of 10.15 radius and the cutter being used is diameter 20.0. If a Wear or Geometry TR Comp radius of 10.15 or greater (when part coordinates programming is employed) so as not to cut the overall feature out of tolerance, a TNRC Interference alarm will be raised.

Similarly, if Centre Line programming was being used, with a 10.0mm radius cutter specified when creating the program, the Concave Radius feature will now appear in the program as a 0.15 radius Concave Feature. If a TR Comp value of 0.15 or greater is used, the same TR Comp alarm will be raised as in the example using Part Coordinate programming.

When using Centre Line programming, plus TR Comp, the TR Comp value can become a Minus Value when adjusting the size of the feature. When Minus Values are used as the TR Comp value, the TR Comp "G" Code is effectively flipped; the Control sees G41 as G42 and visa versa.

Regards,

Bill
 








 
Back
Top