Need Help!- Overcutting, cutter comp, Fanuc Oi.

[LPE Ltd]

Hi, im new to the site.
Im getting an what appears to be an overcut and its doing my head in.
Im trying simply to put a 5mm chamfer on the ends of a 47x20 block, 0/0 ref about center, but on the first chamfer im getting a scallop. Im starting at X-45, Y-50 just to make sure out of any radius interference. Feed to depth then using
G1 G41 X-18.5 D11 (correct tool number and radius offsets);
Y-10;
X-23.5 Y-5;
Y5;
X-18.5 Y10;
G40......

Please could anyone show me what silly mistake im making or point me in the right direction if its a little bit more involved.
Thanks.
Ian.

[underdog]

Ian,

I didn't go thru the actual dimensions you gave but most G41 issues are caused by a few factors. The first move that incorporates the cutter comp MUST come to its end off the part and the last move where the G40 kicks off the CC must also end off the part. In the begin and end the CC must be effective before the cutter touches the part since the move onthe G41 line is a mixture of the programmed move and some extra movement to account for half the cutter or its wear value whichever your offset contains.

Said another way, write your code with two lead in lines and two lead out lines. They can be lines end to end. Make sure they are at least as long a move as the cutter diameter (you may be able to shorten this later- the machine will fault if it is too small - its usually faluts at cutter diameter or cutter radius or at the wear comp value (.006 or so)).

Then with your two lead in lines and two lead out lines, put the G41 D11 on the FIRST of the two lead in lines and G40 on the second (or last) lead out line.

[sinha_nsit]

Your program appears to be OK, except that at the start point you will not get a sharp corner.
Possibly, D11 register has higher radius value (It is radius value, not diameter).

[LPE Ltd]

Hi Underdog, Sinha,

Thanks, ive just changed it slightly to start well away +1.5x cutter diameter just to be sure, unfotunateley i cant finish so far due to the jaws, but i have changed the G40 to mirror the in path. Double checked the offsets and they are correct. Now i have a scallop on both chamfers.

Verbally my program feeds to depth in a -X and -Y quadrant,
applies cutter comp G41 in +X direction
moves towards the first corner of the chamfer, OH!, what a muppet, i see what you mean now, im trying to cut a sharp 'internal' corner with a round cutter as it were? Its never going to work.. Ill extend the chamfer to start in air and that should solve it.

Thanks again,
I have another problem or rather bad understanding which involves applying cutter comp in the Z (G19) plane but i need to get my head around it again first and it may well be similar mistake as i have made above.
Ian.

[sinha_nsit]

Originally Posted by LPE Ltd ... im trying to cut a sharp 'internal' corner with a round cutter as it were? Its never going to work.. Ill extend the chamfer to start in air and that should solve it. ...

Exactly.
Do the same at the end point also.

[LPE Ltd]

Works a treat now....Thank-you.

Two years ive been working on these machines, just goes to show, something as simple as this, you get so invloved with complicated reasoning and you dont see the obvious.

[sinha_nsit]

You are welcome.
Incidently, on Fanuc, you do not need two start-up moves.

[LPE Ltd]

Ill remember that, the 2 works ok on this due to the small part being in the centre of soft jaws and its only a small number off.

Ill try and have a look at the other problem over the weekend if i get chance, its one that i have tried many different ways but failed to get it right or work out why. The one you have have just made clear i had manually got round it without cutter comp but still didnt make the now obvious connection.

[sinha_nsit]

In radius compensation, take care of a few things:
1. The machine will not do something which is mathematically not possible (Make a sketch of the toolpath to observe any inconsistency)
2. For compensation in XY-plane (say), there should not be two (or more) consecutive non-movement commands in XY-plane (macro statements are not counted for this purpose).
3. You cannot switch compensation plane without first cancelling the current compensation mode.

[LPE Ltd]

Ok, ill look at the other problem again as soon as i can with those in mind, and without being presumtuous, maybe you could have a look at the other one, its a bit more challenging, i hope!

[sinha_nsit]

Your second problem is not very clearly explained.

[LPE Ltd]

Ok, I was trying to mill a simple slot with a radius in and out in the z plane ie for example say a 30mm long slot with a 30mm radius either end using a 10mm ball nose. Like a stretched 1/2 pipe.

I used a simple program starting without cutter comp (in the air). i.e

T.....
G1 Z0 F100
G91;
G1 X10;
G02 X30 Z-30 R30; ( i think its G2 not G3 for the ZX)
G1 X30;
G02 X30 Z30 R30;
G90;
G0.....

This produced movement in the Y axis as well (all 3 axis) and linear motion in Z&X during the G02 part,

I then tried it using the G18 command and this seemed to cure it.

However when i tried appling cutter comp in a vertical motion ( as per a reference book example, Peter Smid) it applies it in the Z axis as well so i would end up being 5mm above or below depending on G42 or G41 where i need to be.

I tried reading up on it and understood it that it should work in the G18 plane as long as the G02/03 command states the movement in the X and Z axis only.

I tried my usual method of trying different combinations to work it out but i couldnt get it right and ended up fudging it with no comp.

In the tool selection (Fanuc Oi-m) i selected Ball nose and used 5mm as the cutter radius, but im not sure if thats correct because if i change it to an F end mill it seems makes no difference to the actual resulting positions after each block., Ive tried it also with arc modifiers and the results are the same.

When a ball nose is selected, should i enter the complete cutter diameter in the geometry 10mm or 5mm?

Ill try it again when the machines free but i would appreciate any guidance.

Thanks
Ian.