Help needed - Eia control of chamfer tool driving too deep

Hi all

Hopefully someone can point me in the right direction...

I am running the VQC with M2 Control in drip feed mode which I have been doing for a while and all has been going as well as can be expected.

I'm using Bobcad for my Cad/ Cam and that has been working fine too.

The exception is when I try and do a chamfer. I am setting a very small edge break - 0.2mm but the tool is driving in deeper and giving me a 3mm chamfer.. I manually adjusted the Gcode to only drive in 0.2 from the top (so ignoring the 45 degree section on the tool) and it gave me the desired results in the simulation and on the part. The Chamfer is the last op and essentially junking the part.


I carried out a trial in the Cam tonight. I set up a basic cube with a small chamfer and the G code is coming out as I expect and putting the tool tip where it should be. The simulation (both Bobcad and 3rd party) are showing it is sending the right commands.. so I am confident the cam is giving all the right commands and positioning the tool to compensate for position, and instructing the depth to accommodate the offset. (I analysed the code for the part and it looks fine too)

The code below is the trial piece I mentioned above. It is a 0.141mm deep Chamfer (0.2mm flat on chamfer) on a 50x50mm square block with Zero point set in the middle of the top surface. I have set the tool to be 1mm from the edge of the part, which also means it goes down 1mm before it engages the part. Total depth of tool tip is thus -1.141mm from datum (underlined below).

%
O200 (CHAMFER TEST.EIA)
(SAT. 02/18/2017 09:21PM)
( MAZATROL CAM M-2)
( T1 CHAMFER MILL , DIAMETER = 20. , LENGTH = 127.)
G90 G80 G40 G49 G17 G94 G00
(Machine Setup - 1 Chamfer Mill)
(FEATURE 2 AXIS)
T01 M39
M06
( T01)
S3000 M03
G54 G90 X26. Y-26.
G43 Z25.4 M08
Z5.08
Z2.54
G01 Z-1.141 F109.537
X-26. F219.075
Y26.
X26.
Y-26.
G00 Z5.08
Z25.4
M09
M05
G91 G28 Z0.
G91 G28 Y0.
M02
M30
%

So next I start to think I have some form of compensation going on in the CNC... I checked this and it is set to Zero in the Tool Data page (as I had entered). In addition, I assigned the tool as an endmill to emulate the same characteristics of an endmill as the endmills are working perfectly. The Gcode doesn't care what tool is actually in the pocket as long as it has a tool offset it does whatever the code is programmed to do. The problem still occurred.

I tried a different tool and checked the tool length offset/ remeasured tool length etc, but that all looks ok.

I also checked the tool offset page and they are all zero as well (never entered anything in these cells)

I'm thinking there may be another parameter that I am missing or an compensation somewhere that is pushing the tool into the workpiece.

Id prefer to not have to manually adjust code to accommodate for something that should be an easy fix.

Any ideas are much appreciated.

Cheers

Mick

It's all in the CAM if you're running tool comp. In the computer.

I'd check that you have your tool set up right in CAM.

There should be some tip offset, so it's not cutting right on the point. And there will also be a small flat spot (generally) on the tip of your tool, so you need to check that's right too.

From what i can see if your code, the controller won't care what the tool is. It's just tool 1 with the z offset that you've taught it.


Sent from my LG-H815 using Tapatalk

Sorry just read the whole thing...

So if you run that program with a flat end mill do you get a 1.141mm step cut in the edge?

Sent from my LG-H815 using Tapatalk

xa-mont said:

It's all in the CAM if you're running tool comp. In the computer.

I'd check that you have your tool set up right in CAM.

There should be some tip offset, so it's not cutting right on the point. And there will also be a small flat spot (generally) on the tip of your tool, so you need to check that's right too.

From what i can see if your code, the controller won't care what the tool is. It's just tool 1 with the z offset that you've taught it.


Sent from my LG-H815 using Tapatalk

Click to expand...

Thanks for the prompt response.

That's what I thought initially as well and I'll check again to make sure I didn't miss something, although the code looks correct unless there is something going on with G43....

With the software, you enter the tool data (Diameter, pointed or not, number of flutes, left, right or no compensation, angle of chamfer tool, depth, offset, chamfer angle etc). It works out the rest. I do enter a tip offset, and that is the 1mm I mentioned in the example above.

With that in mind, as it is walking the centre of the tool around the part, as we are chamfering, it shouldn't matter if I am using a 6mm or 20mm chamfer tool (pointed ones)as the contact point of the part and the tool tip path are still the same to my reasoning. I use the same offset for both tools for the purposes of the test.

xa-mont said:

Sorry just read the whole thing...

So if you run that program with a flat end mill do you get a 1.141mm step cut in the edge?

Sent from my LG-H815 using Tapatalk

Click to expand...

The cam offsets the tool further so the cutting edge is in contact.

This code is the same job but the tool but has a 10mm flat on the bottom. You can see the X&Y are now pushed out a further 5mm (31mm vs 26mm). Depth has stayed the same.

%
O200 (CHAMFER TEST.EIA)
(SAT. 02/18/2017 10:14PM)
( MAZATROL CAM M-2)
( T1 CHAMFER MILL , DIAMETER = 20. , LENGTH = 127.)
G90 G80 G40 G49 G17 G94 G00
(Machine Setup - 1 Chamfer Mill)
(FEATURE 2 AXIS)
T01 M39
M06
( T01)
S3000 M03
G54 G90 X31. Y-31.
G43 Z25.4 M08
Z5.08
Z2.54
G01 Z-1.141 F109.537
X-31. F219.075
Y31.
X31.
Y-31.
G00 Z5.08
Z25.4
M09
M05
G91 G28 Z0.
G91 G28 Y0.
M02
M30
%

I'll do up a quick one the same in fusion with my post and see what we get.

Sent from my LG-H815 using Tapatalk

I'll check the tool tip reference position on the machine again tomorrow... maybe something has gone awry....

Ill check zero with the tool that I set zero with then try the tip of the chamfer tool on the same reference point... I would expect they are both the same if the tool offsets are working properly...

heres what i get. this is using a 20mm 45deg tool with 5mm flat on it.

O1001
(T1 D=20. CR=0. TAPER=45DEG - ZMIN=-2.141 - CHAMFER MILL)
G90 G94 G17 G49 G40 G80
G28 G91 Z0.
G90

(2D CHAMFER1)
T1 M06
M39
S3000 M03
G54
M08
G00 X0. Y-30.5
G43 Z15. H01
G00 Z5.
G01 Z2. F1000.
Z-2.141 F333.
Y-28.5 F1000.
X-25.
G02 X-28.5 Y-25. J3.5
G01 Y25.
G02 X-25. Y28.5 I3.5
G01 X25.
G02 X28.5 Y25. J-3.5
G01 Y-25.
G02 X25. Y-28.5 I-3.5
G01 X0.
Y-30.5
G00 Z15.

M09
G28 G91 Z0.
G28 X0. Y0.
M30
%

heres what it looks like in relation to the corner of the part.

Thanks for doing that . Thats what mine looks like on the screen as well. Will try a few things this morning and see what i can find

Sent from my SM-G930F using Tapatalk

Ok looks like I found my problem.

I set the datum on the work piece with the tool I use for 99% of the process. Unfortunately, the tool length offset wasn't set properly (approx. 2mm out) and when the chamfer tool came in (at the correct Tool offset)it actually went deeper into the job.

Going to run a part this morning and see if it works.

As usual in this game, User error is the is 99% of the problem

sophtayl said:

Ok looks like I found my problem.

I set the datum on the work piece with the tool I use for 99% of the process. Unfortunately, the tool length offset wasn't set properly (approx. 2mm out) and when the chamfer tool came in (at the correct Tool offset)it actually went deeper into the job.

Going to run a part this morning and see if it works.

As usual in this game, User error is the is 99% of the problem

Click to expand...

It's all learning though

I rapided a 4 flute indexable 25mm end mill through 10mm steel plate on Friday night... It stalled out my mazak (first time I've done that)... I had my feed plane at the bottom of the part [emoji14]

Won't make that mistake again. Suprisingly the inserts and cutter were still perfectly fine.

Sent from my LG-H815 using Tapatalk

Ouch... i would heart crapped myself

Sent from my SM-G930F using Tapatalk

sophtayl said:

Ouch... i would heart crapped myself

Sent from my SM-G930F using Tapatalk

Click to expand...

Didn't help that i was a few beers in (930pm on a Friday, the client just happened to see a fork lift driver who had just been at my factory heading back to his lot and asked if he knew anyone that could do the job asap), had like 5 mates around heckling me and the 2 clients standing over my shoulder [emoji14]

Sent from my LG-H815 using Tapatalk

xa-mont said:

Didn't help that i was a few beers in (930pm on a Friday, the client just happened to see a fork lift driver who had just been at my factory heading back to his lot and asked if he knew anyone that could do the job asap), had like 5 mates around heckling me and the 2 clients standing over my shoulder [emoji14]

Sent from my LG-H815 using Tapatalk

Click to expand...

It's amazing the dumb little routine details you can miss when there's a crowd to distract you.
I rarely let my friends hang around the shop when I'm running a new program or a complex setup.

cwtoyota said:

It's amazing the dumb little routine details you can miss when there's a crowd to distract you.
I rarely let my friends hang around the shop when I'm running a new program or a complex setup.

Click to expand...

It wasn't really planned, but it all worked out in the end.

Sent from my LG-H815 using Tapatalk

Quick update. There was more to it as well. I had the air pressure turned down and i wasnt getting consisted tool offsets on the measuring tool. Im assuming the tiol clamp wasnt pulling hard enough. Upped the pressure and looks to be ok now.

Oh the joys

Sent from my SM-G930F using Tapatalk

sophtayl said:

Quick update. There was more to it as well. I had the air pressure turned down and i wasnt getting consisted tool offsets on the measuring tool. Im assuming the tiol clamp wasnt pulling hard enough. Upped the pressure and looks to be ok now.

Oh the joys

Sent from my SM-G930F using Tapatalk

Click to expand...

There should be a Reed switch/inductive sensor to tell the machine when a tool is clamped or not. It's up in the covered section around the spindle. There's 2 right next to each other (clamp/unclamped) maybe make sure they're right cause you probably don't want to be milling without your tool pulled up properly.



Sent from my LG-H815 using Tapatalk

I just checked them but cant see any leds. The striker is covering the upper sensor by about 3/4. I would hazard a guess that the tool clamp sensor would give me a fault it it didnt make home?

Sent from my SM-G930F using Tapatalk

I had the air pressure down to 300kpa but have it back up to 600kpa since this morning and so far so good.

Sent from my SM-G930F using Tapatalk

sophtayl said:

I just checked them but cant see any leds. The striker is covering the upper sensor by about 3/4. I would hazard a guess that the tool clamp sensor would give me a fault it it didnt make home?

Sent from my SM-G930F using Tapatalk

Click to expand...

Yeah pretty sure it does. I reset the position of mine because it wasn't completely when tool changing and just ripping the tools out with the tool changer... Not such a good way to do things.

Sent from my LG-H815 using Tapatalk