[jrm850]

While milling some uhmw on Sunday the mill freaked out and tried to drive a 1/2 endmill directly through the center of a 3d profile. This happened immediately after it was finished with a hogging profile and should have switched to a 1/4" ball before it started a waterline rough. In addition to driving the mill into the part from the Y side, the x axis was making bizzarre sounds and the zero ended up with a 3" discrepancy after the accident.

The code was generated in CamBam and tested in cutviewer without problems or rapid crash errors. The mill is a series 3 1100.

After this crash, I cut air using the same code and it did the exact same thing in the exact same section of code. (between operation 1 and 2)I ended up running each operation independently to finish the part. Operation 1 and 2 cut perfectly, but Mach3 balked at operation 3 disconnecting from the mill and flashing a driver error. If that was the problem, it doesn't make sense to me why the crash would happen between mop 1 and 2 instead of between 2 and 3. Now I am a little gun shy. Thank god it was only uhmw and not my vise.

The final operation was a scanline finish pass with a very short stepover and the file generated was over 15mb. The Controller is a stock Tormach PC with Mach3. Could this be a RAM error?



The problem started right after the last G3 was finished. The stock was x4",y4", z3. There is a 2.677" diameter circle polyline centered on the 4x4 block that was set as internal boundry. It plunged to about z-2" and then headed straight for the center of the stock (2,2). Target depth was only 1.684"

Any help will be greatly appreciated.

G0 X1.2777 Y3.426
G0 Z-1.548
G1 F44.0 Z-1.684
G3 F88.0 X1.2008 Y3.3843 I0.7223 J-1.426
G3 Y0.6157 I0.7992 J-1.3843
G3 X3.5985 Y2.0 I0.7993 J1.3843
G3 X1.2777 Y3.426 I-1.5985 J0.0
( 3DSurface1 )
G0 Z0.125
( T7 : 0.25 )
( Tool Taper coming soon )
( TOOL/MILL,0.25,0.125,0.0,0 )
T7 M6
M3 S5100
G0 X2.0485 Y2.028
G0 Z0.02
G1 F39.0 Z-0.04
G3 F79.0 X2.048 Y2.0146 I0.523 J-0.0271
G3 X2.0485 Y1.9719 I0.5159 J-0.0154

[Scott_M]

There is no height offset data in your code. It still thinks it is using the same length tool as op 1. Your T7 M6 line should read M6 T7 G43 H7. then it will get the height info from the tool table. Assuming you have set that up.

Scott

[jrm850]

There is no height offset data in your code. It still thinks it is using the same length tool as op 1. Your T7 M6 line should read M6 T7 G43 H7. then it will get the height info from the tool table. Assuming you have set that up.

Scott

I did not have it set up for tool offsets. I was just going to re-zero z after it paused for the tool change, but it never got that far.

[Steve Seebold]

I did not have it set up for tool offsets. I was just going to re-zero z after it paused for the tool change, but it never got that far.

ALL tool length offsets need to me set before you push the start button. It
may not be a requirement with the Mach operating system, but it's a really good habit to get in to. It will prevent problems like this.

[jrm850]

Would not having the tool offset set cause a full speed Y crash into the part? I doesn't seem logical to me but I am a noob to cnc and definitely do not know everything... yet

ALL tool length offsets need to me set befort you push the start button. It
may not be a requirement with the Mach operating system, but it's a really good habit to get in to. It will prevent problems like this.

[twocik]

Why even risk the crash ... I saw issues like this when I first setup the machine without the tool values. I was trying to zero each tool for each mop, for some reason you get errors like this and just be glad you didn't crash into your brand new vise, table, etc.. not to mention if you're using premium tooling. It can be a pain to reset these values over and over for single part runs, but like Steve said it's very good practice. Don't forget every time you crash it's a good idea to re-check everything (parallelism, shaft couplings, backlash, etc..). A bad enough crash will sometimes loosen and put your machine out of spec.

[Steve Seebold]

Would not having the tool offset set cause a full speed Y crash into the part? I doesn't seem logical to me but I am a noob to cnc and definitely do not know everything... yet

No, not having your tool length off sets done properly will not cause you to crash the Y axis into the part.

If you would like, send me a PM where I can send you my phone number and I will talk you through a set up and I'll stay on the phone with you until you have your part running.

I'm going boating Tuesday, Thursday and Saturday morning, but I'll be home after about 3:00 PM pacific time. I race remote control gasoline powered model boats and I have a race this Sunday, and I have only had a boat in the water 3 times in the last 3 years. I need all the practice I can get.

I don't want to go out and wreck someone else' boat.

These aren't my boats, but it will give you an idea what I'm talking about.

[jrm850]

It seems like a consensus then, I appreciate the advice. I think tomorrow I will add the offsets and run it again in the air to see if it was the culprit.

Thanks again,

Jeff

[Scott_M]

Hi Jeff

Don't forget to edit your code. the code you posted did not call for the offset. A M6 should include or be followed by a G43 ( apply tool offset )
example for tool 2

M6 T2 G43 H2
M3 S2500

or

M6 T2
G43 H2
M3 S2500

Hope that helps

Scott

[jrm850]

Nice Boats! Looks like a lot of fun. I've had the RC heli bug in the past and used to make some airboats out of my crashed planes as a kid, but I've never had the opportunity to own or drive anything like that.

I appreciate the kind offer but I already finished the part. I'll PM you my information anyway and definitely take you up on it next time.

Thanks again,
Jeff

No, not having your tool length off sets done properly will not cause you to crash the Y axis into the part.

If you would like, send me a PM where I can send you my phone number and I will talk you through a set up and I'll stay on the phone with you until you have your part running.

I'm going boating Tuesday, Thursday and Saturday morning, but I'll be home after about 3:00 PM pacific time. I race remote control gasoline powered model boats and I have a race this Sunday, and I have only had a boat in the water 3 times in the last 3 years. I need all the practice I can get.

I don't want to go out and wreck someone else' boat.

These aren't my boats, but it will give you an idea what I'm talking about.

[jrm850]

I've been relying on CAM to generate the code and the offsets, but I'm starting to get a bit more comfortable reading the code and making minor edits in Mach3. One of the reasons I got lazy on this project is having to synchronize the tool libraries for mach3 and the CAM program. Thank you for the example. I either need to aquire more tool holders or keep learning

Hi Jeff

Don't forget to edit your code. the code you posted did not call for the offset. A M6 should include or be followed by a G43 ( apply tool offset )
example for tool 2

M6 T2 G43 H2
M3 S2500

or

M6 T2
G43 H2
M3 S2500

Hope that helps

Scott

[Steve Seebold]

I've been relying on CAM to generate the code and the offsets, but I'm starting to get a bit more comfortable reading the code and making minor edits in Mach3. One of the reasons I got lazy on this project is having to synchronize the tool libraries for mach3 and the CAM program. Thank you for the example. I either need to aquire more tool holders or keep learning

Your CAM will generate your motion commands ant tell the machine which offset numbers and and work shift offset numbets, but you have to establish your own tool length and work shift offsets.

The first few lines of your program should look something like this at each tool change: (this is my way, someone else might have a different idea)

N1G17G80G40
G54
T1M6
( TOOL 1: .25 CUSTOM )
S4500M3
G90G0X and Y start point
G43Z1.H1
M8

[jrm850]

Are you saying that I only have to worry about the tool library and offsets in the Cam program or does mach3 need to have the same tools and offsets? I've been mirroring the libraries in both to this point.

Your CAM will generate your motion commands ant tell the machine which offset numbers and and work shift offset numbets, but you have to establish your own tool length and work shift offsets.

The first few lines of your program should look something like this at each tool change: (this is my way, someone else might have a different idea)

N1G17G80G40
G54
T1M6
( TOOL 1: .25 CUSTOM )
S4500M3
G90G0X and Y start point
G43Z1.H1
M8

[rowbare]

The CAM program needs to know the tool diameters for each tool so that it can calculate its paths etc... The accessible CAM tools (i.e. not mega$$$) I use don't care about lengths. You set your length offsets in Mach.

Have you seen Tormach's tool table videos? They do a great job of explaining tool length offsets. [ame=http://www.youtube.com/watch?v=_8apTgMTvjI]How to Change Tools in Mach3 CNC - Part 1 - YouTube[/ame]

GWizard has pretty good tool management capabilities and can export tool tables though I am not sure how to import them into Mach.

bpb