Drill hole for G41/G42 path & feed control

I have two question for the community...

I have the machine always working with G42 or G41 so with radius compensation, i have find some awkward problems using this method, first is my cutting bit do not plunge in, i have to use a separate drill tool to plunge, then my bit will go inside the hole made from the drill and start cutting from there.

Now since i work with radius compensation the position at which the bit will plunge in is very random, so i cannot calculate where to make the drill hole.

The system i'm using now is making the bit G-code with radius compensation, start and write down the plunge in position, then stop, make a plunge in G-code for my drill in the position that i wrote down.

I would like to know if anyone has come up with a better solution to plunge in the G41/G42 start position.

Other question i have for the G42/G41 mode, does EMC2 provide a solution for feed rate optimization for curved path sections, like the Siemens functions CFTCP, CFC, CFIN.

The problem is that on curved paths the machine has to either slow down or accelerate to maintain a constant peripheral speed, on lines the problem does not occur, but on curves peripheral speed and tool trajectory speed are very very different, EMC2 take in consideration only the tool center trajectory, it does not take in count the peripheral trajectory for what i have seen, so i was wondering if there is a solution to regulate speed according to the peripheral path.

No right now it does not happen, i'll try to explain why with a picture



EMC2 for what i have seen, when you load a programmed path with G42 it displays the G42 path and it's regulating the speed according to the G42 path.

Now let's say we are doing this simple program at feed 1000, on linear paths the programmed path and the G42 path do not differ so you have same speed on both path, but on curved path like the radius 50 the paths are different, for the G42 path the travel length is 47.1mm (30*6.28/4) for the programmed path the travel is 78.5mm (50*6.28/4), this means that when you keep a constant feed of 1000 on the G42 path, the speed on the programmed path (peripheral path) is 1.666 times faster (78.5/47.1) so you are actually going at feed 1666 (1000*1.666) because you are moving and keeping constant speed on the small radius but actually cutting on the big one.

Now in my example the ratio is just 1.666, but think about a radius 82 done with a 160 diameter tool, the ratio is huge the speed difference will be huge and the job will not be done properly.

As for the plunge in problem, what i meant for random is, i can't predict where the plunge in will be calculated to be with G42 path calculation, but once the G-code has been played the position will not change on that G-code, still it's not enough for me because i need to know that position precisely before i start the bit program, to make the drill program.

The drill program does not have radius compensation, only the bit program does.

What i want to do is make a cutting program with radius compensation for the bit, and then make the drill program to drill a hole where the bit has to plunge in, then play on the machine the drill program first that will make me the hole, and then the bit program that will enter the drilled hole and start cutting.

The problem is, how do i find the plunge in position of the bit precisely, so that i can program the drill in the correct position?
My solution is to play the bit program and see where it plunges, but it's not good because i need to program everything before starting the machine.

grandixximo wrote:

No right now it does not happen, i'll try to explain why with a picture

EMC2 for what i have seen, when you load a programmed path with G42 it displays the G42 path and it's regulating the speed according to the G42 path.

I am not an industry expert, but this whole concept seems TOTALLY wrong!

The main feature of G41/G42 is to make the programmed path specify the periphery of the tool, not the center.
And, it only makes sense when the tool is moving in XY. Drilling, on the other hand, would always be
specifying the center of the drill bit, and you don't move in XY while drilling.

So, as others have said, it is standard practice to exit the radius offset mode when drilling, and only use
it when side milling.

I can easily see why you can get somewhat unpredictable hole locations when leaving the offsets on.

(Of course, one way to fix this is to set the tool table diameter for the drill to zero, then there will be no offset.)

Jon

The feed concept is correct as desired by the OP. Cutter comp (G41,G42) is a tool so to speak for the programmer. The concept when used as designed way back was this. The programmer can generate code based on a zero diameter mill, so programmer codes the profile of the part. Then when the machinist sets up the machine, he would enter the diameter of the cutter and the control will do the math to offset the path properly. This allows several things. The machinists can use any size mill as long os its not bigger then the smallest inside radius. machinist can correct for tool dulling without the need to bother the programmer. different size mills can be used for the rough and finish path with the same code by simply changing the dia.

One of the things the control is also supposed to do is adjust the feed rate to match the programed feed at the cut surface, not the tool path. If EMC does not do this, it would seem like a fundamental flaw to me. Not one that bothers myself as I almost never use cutter comp. for general purpose stuff which I mostly do, its not an issue. But if I were cutting say plastic, that slow corner may melt the plastic as the chip load will go way down and the heat will stay in the part.

As for predicting where the hole needs to be drilled, OP needs to make that NOT random. You need to know where to start cutting before you turn on comp. that should be where your hole is.

@jmelson

You totally misunderstand me, i never said i drill with radius compensation, if i did i'm sorry my mistake, in fact drilling with radius compensation it's impossible, i never even tried it since i think it's impossible.
What i meant is, i have my side miller working with radius comp, but my side miller does not drill, so i have to make a hole with a drill before so that i can go down freely trough the hole with my side miller, my problem is that with radius compensation i cannot predict where the miller is gonna go down, therefore i cannot make the program for the drill.
I d not have radius comp on the drill program, i just cannot program the drill without knowing exactly where to make the hole for the mill.

@btvpimill

I totally agree with the first part of your post, not adjusting the feed rate to match the programmed feed at the cut surface, it's a fundamental flaw, not only when working plastic, but all other kind of material, what i'm doing is polishing granite, you can only imagine what the machine does on corners, it's ridiculous and dangerous...

As for the plunge in, it seems that you never worked with radius compensation in EMC...

www.linuxcnc.org/docview/html/gcode_tool...l#cap:Inside-Profile

Observe the last g-code in this page, as you can see the Z-1 it's after the G41, and there is no other way to do it, because you need a lead in move longer then the radius of the tool, and you must do it in G0 outside or over the piece you are working, unless you can think of a better solution.

@BigJohnT

See this G-code



If you play it on EMC you can see where the machine will plunge in, and understand what i mean for it's random, i could say it's unpredictable....

I'm following almost to the letter the example that is show on the linked page above, the problem is that as you say the lead in when progressing into a cutter comp profile will depend on your start point and the side of the line you start your lead in move, as you see in the g-code i have to plunge at the beginning of the lead in, so it's difficult to predict this position unless you know exactly how EMC calculate the lead in move, and still it will get some thinking.

I apologize for the use of the word random, it maybe exaggerated, but i think i can freely say that it's hard to predict where the side miller is gonna go down.

grandixximo wrote:

@jmelson

You totally misunderstand me, i never said i drill with radius compensation, if i did i'm sorry my mistake, in fact drilling with radius compensation it's impossible, i never even tried it since i think it's impossible.
What i meant is, i have my side miller working with radius comp, but my side miller does not drill, so i have to make a hole with a drill before so that i can go down freely trough the hole with my side miller, my problem is that with radius compensation i cannot predict where the miller is gonna go down, therefore i cannot make the program for the drill.
I d not have radius comp on the drill program, i just cannot program the drill without knowing exactly where to make the hole for the mill.

Ahh, that is different. Well, it is usually assumed that when using G41/G42, you have an approximate idea
of cutter size when creating the program. Therefore, the drilled hole can be put in approximately the right
place so that the milling cutter doesn't have to hog into large amounts of stock. As you say, you can't know the EXACT
path of the cutting tool due to different tool diameters being entered, but the whole idea is to reduce the amount
of material to be removed by the milling cutter. So, this shouldn't be a "random" problem, just an approximation
problem.

Jon