Brother Speedio drill program acting differently/wrong

[gustafson]

So
2021 Speedio s700X2
The program originated in fusion CAD/CAM
proven program, stored in machine
hundreds of parts run, in several runs over several months
One day it up and cleans off a .406 drill
Now since the part is held down by a couple 1/4 SHC I have had to mod some moves on occasion and later modded it to run multiple locations
SO I fix the program and off I go.
Happens again on another program
Ok, I go through all the programs I can see for similar parts[I run dozens of similar parts] and fix them by inserting a G00 Z.9 or something.
fast forward to today
First I run a part that I still have labelled as test so not truly proven although I have probably made good parts with it
the second half of a hole pattern are not all the way through. Ok, maybe it isn't quite right, only need a couple, figure it out later
I go to run the program that initially had a problem a few weeks ago.
Now it drills this second half of the hole pattern not all the way through
This it the subroutine for the hole drilling. There is a tool call and G52[offset from previously defined g54] and call this subroutine. 3 times 3 parts. First 5 holes drill fine, second 5, shallow
There is a SHC screw between the holes at lines 1105 and 1108, thus the G00 Z.899 move, have to kill the G81 and redefine it

So, WTF!
NOw if you tell me the code is wrong, ok, fine, I fix it
But then, why the FOOOK did it run for months before?

Look, I am new to G Code, I have used Heidenhain for 30 years, and if you write a program in heidenhain, it runs, it will run, for 30 years.

 

[DavidScott]

I don't see you calling out either a G98 or G99.

 

[gkoenig]

This it the subroutine for the hole drilling. There is a tool call and G52[offset from previously defined g54] and call this subroutine. 3 times 3 parts. First 5 holes drill fine, second 5, shallow

Why? Just spit the whole program out in CAM and be done with it. This isn't the days of 256kb of memory; what is the gain in adding sub program complexity to anything?

How is it killing drills? Not retracting out of the hole before moving in XY towards the next one? Or drilling too deep?

I would run the program in air, single block. Brothers are not perfect, but I've never seen one execute code "wrong," they always do exactly what you tell them. That is why the admonishment about sub programs; they just make finding issues like this more complicated than they would otherwise.

 

[Spruewell]

Is the drill slipping in the holder?

 

[gustafson]

So sorry busy couple days, didn't have time to post
I am not imagining things
Last night I ran another program and blew up a countersink
same fixture, same setup, no change in tools from previous parts
.5 inch thick blank. Zero bottom of blank/top of fixture
.5 diameter 90 degree mill
previously milled .312 flange
part held down with two 1/4 SHC at x-1.113, Y-.87//X1.113, Y.87 on .5 section
Block 1159 correctly countersinks to size on .5 blank
Block 1162 correctly deburrs .406 hole in .312 thick section
Tool wipes out SHC at x-1.113 y-.87 on the way by
fixture was not removed from machine. Tools not removed from machine.

I previously ran perhaps three of these parts a few weeks ago.
Since the flange is the correct thickness, and the first two countersinks are correct, the tool lengths and fixture height must be correct

Her comes the fun part:
it was 5PM, I swear a bit and shut off the machine and go home
Come in this morning and warm the machine up.
I have not unbolted the part from the machine as it is salvagable


I run the program from the start of that cycle.
NOw I am not sure how all machines run but on the Brother it loads the previous tool at the previous spot before the tool call, stops and you hit cycle start and it goes.
The [still damaged tool] is no where near the screw
OK, OK what have I changed?
I am running it with the feed knob down, and the Brother does not interpolate rapids[Heidenhain interpolates everything] so even though the screw is in no way in a line between the two holes, the non interpolated rapid means it moves towards the screw in rapid[much shorter x move is made faster]
But I run it single block and stop it , it is up high enough and clear of the screw.
Run it at full speed no problem.
Run another part, runs fine

This is a single location program, the only thing not straight out of CAM is the G52, it is run as written. Maybe I deleted spurious G54 calls that I have not figured out how to remove in the post yet.
On the next part I ran, the only thing I changed was running the .406 hole deeper as it was not quite all the way through.

Mind you this is not a detail thing, it did not just ding the screw on the way by, it tried to machine off a chunk of the screw head, and there is a screw head sized piece of the tool missing

I am sure I am missing something, but this sure don't seem right.

 

[gustafson]

Actually I might have changed block 1161 manually weeks back to add the z .94 but I do not recall, nothing changed today

 

[gkoenig]

I am running it with the feed knob down, and the Brother does not interpolate rapids[Heidenhain interpolates everything] so even though the screw is in no way in a line between the two holes, the non interpolated rapid means it moves towards the screw in rapid[much shorter x move is made faster]

User Parameters
Switch 1
#0172 Interpolation

Switch to Type 1 or Type 2 and the machine will interpolate rapids. It will not interpolate rapids on the G100 tool change though (those will always dogleg because of the axis decomposition where the XY moves get executed before Z).

 

[gustafson]

User Parameters
Switch 1
#0172 Interpolation

Switch to Type 1 or Type 2 and the machine will interpolate rapids. It will not interpolate rapids on the G100 tool change though (those will always dogleg because of the axis decomposition where the XY moves get executed before Z).

Thanks
May have to change that. It's nice to know where the machine is going when you tell it to go.

 

[alphonso]

Blocks 1161,1165,1168. I usually do a Z move by itself before XY move.

 

[Omega]

Get rid of those Z moves before the drill cycle (and after), G43 Z.99 H? in main then G98G83 X Y Z Q R.1 to rapid to .100 above part or where ever you want drill to start drilling from.
If you want the drill to stay down to .100 use G99