how does G41 work exactly?

[max90272]

Hello,
I 'm a little bit confused with cutter compensation G41 (for climb milling) g code?

When using cutter comp in any CAM software, I noticed that the G41 and the D value is outputted only on finish passes... which will result in a lot of G41 and G40 codes within the same tool. In some cases, the controller of the CNC machine (for instance Hass VF2) doesn't like that. It will stop and create an alarm in a lot of cases. However, If I remove all the g41 and D values manually, and insert only 1one G41 D# at the beginning of the tool change, the machine will operate perfectly and WILL compensate perfectly.. So I guess my question is... Why do CAM software bother to output G41 codes only on finish passes if this will create syntax errors down the line on the controller? It seems to me that the software could just output one G41 D# value at the beginning of the tool change and one G40 at the end and everything would work? Not sure if I make sense?? Any thoughts?

thank you

[beege]

Okay,

G41 ISN'T for "climb milling". although for almost all applications it ends up being true. It's "Offset Left of Geometry" If you're working in a CAM system, you can compensate for the radius of the tool there, or at the machine. You've probably let the CAM system compensate for the tool there, and gave a specific diameter for the tool to be used. You could have specified for the compensation to happen at the machine, and chose any number of tool diameters to work with. The entry at the machine for tool radius would have been half the diameter, of course. OK, so you've chose for the CAM system to generate the pass based on a tool diameter. Taking out the G40s means the machine is continuing to compensate for the tool radius (now zero or close) but the errors are miniscule, and probably even non-cutting. Change to a sharpened tool, where your offset value starts to get larger (-.030?) and your G40-less contours start to gouge your part. because the machine is still compensating to the LEFT of the line which was supposed to be non-cutting. I'd leave them in to be safe. It doesn't hurt, and is what you've asked for your CAM system to do.

[Eurisko]

The controller shouldn't have problems with multiple G41 Dnn calls, provided :

G01 G40 Xnnn Ynnn D0 (terminate the G41 code and move to safe position)
And
The tool radius comp does not exceed the initial G01 G41 Dnn Xnnn Ynnn move.

Hass may be an exception, but multiple calls to G41 are used on every machine I've seen, with no problems.

[HuFlungDung]

The CAM software must not be properly set if you see actual alarms due to 'Tool too large' or some such. Each feed sequence needs its own lead in and lead out to the profile when using radius compensation. This is because I believe, in most instances, rapid movements are non-compensated movements, so you'd end up with a bunch of gouges unless the tool is descending, for some reason, by a distance equal to its own radius, from the part profile, wherever it needs to come down.

Now if you are using wear comp as 'machine radius comp' then you'd think different rules apply, because you could theoretically run with zero in wear comp, and successfully complete a toolpath, because an offset of zero should never cause a glitch

[max90272]

Mr. Beege, and others....

OK so let's assume that we do cutter comp. on the CAM system instead of at the machine... so i program my part letting the software know what cutter diameter I am using... for instance 0.500" diameter cutter but in reality the only available cutter is a resharpened one and measures at 0.480"... you would put a 0.020" comp value in the register for that tool # at the machine... wouldn't you want your roughing cuts to be accurate too? It seems to me that if you told your software to leave 0.005 material for finishing and you use a smaller cutter (like above) your finish pass will not be 0.005 but rather 0.015" (0.005 + have diameter discrepancy) and will not be what i wanted? any thoughts?

[HuFlungDung]

I cannot counter that argument, because it sounds like it could be a problem in real life. But keep in mind that during roughing, you will get tool and machine flex that may or may not leave the exact amount to finish. I think the trick is to get repeatable results, do the same thing over and over. If as you say, you find the finish cut is heavier than anticipated, and the part is coming out with material yet to be removed, wouldn't you just tweak the comp amount on the next part so it comes out right?

Often, a person will rough with a larger diameter tool than the finisher, and then you're faced with a significant deviation in every internal corner, because the fillet has more finish allowance than the straightaways.

For most instances, I suppose the best idea is to tell your CAM the truth and tell it you are using a .48 cutter and not a .50 because there will be some adjustments on a complex toolpath, that CAM will make so the program will run without interference alarms. That is, often times, even with full radius comp, the CAM will output a slightly different path than just a duplicate of the geometry on the screen.

However, I can envision some instances where you might want to include a semi-finish, then a finish path, particularly if you have no idea what diameter tool is going to be used. But does that ever happen? Most of us always use a tool that is close to a theoretical ideal size.

I'm curious about how your original program ran with just a G41 called at the beginning with the tool change lines, and cancelled at the end with a G40. I'm having difficulty believing that would run okay and still do the right thing (be on size) all the way from beginning to end. In my mind it would appear that there are too many ways that such a path would result in even more alarms, or simply result in an uncompensated or displaced path. But, I guess if it works, you can do it

[Eurisko]

I'd program the nominal tool size (.500) and use cutter compensation at the control, for roughing, (semi finishing, if needed), and finishing.

I've never liked using the same tool for roughing and finishing. It may save time with tool changes, but it adversely effects tool life and part quality.

btw, most cutter comps tend to be radius comps, not diameter comps.

Is Haas an exception?

[HuFlungDung]

Radius or diameter input is an optional setting in Haas, I believe.