[Rich05]

So far have logged in about 75 hours of running the mill not counting setup times, cleaning etc.

I have been running an IH CNC 3 axis 2hp for about a couple months now. So far have produced some decent parts some of them fairly large 24" with pockets, contouring, various Z-X Z-Y transitions as well. Working with aluminum.

So far so good I guess. No many scrap pieces at all. But I noticed I have destroyed quite a few endmills, and drills. Mabye about 20 total including drills.

A couple time have had the mill grind against or the holder grind down on the part clamps. Lots of times have not set the proper retract for tools or feed planes, many times restarted an operation that was paused forgetting to turn the spindle back on.

Most of endmills destroyed are 1/4-3/8. Never damaged the mill table. Yet. I have been told if I keep it up casastrophic mill damage is not far off! I have no machining background and can not take time to get educated in it or become a journyman. But I am just wondering how typical this destructive track record is, if it will end soon, or what.


These seem to be my most common mistakes.

1- forgetting that top of stock is z= .75 not z=0 (hence drills and endmills crashing in to the part

2- clamps too close to the endmill path or tool holder

3- smacking drills into parts while setting up parts

4- forgetting to turn spindle on when resuming an operation that was terminated with emergency stop (tool crashes into part)

5- Rapid moving mill table in wrong direction crashing into servo casing (forgetting the right direction) this is a problem with the long frame parts where there is no room for error like that while setting up.

6- Forgetting to turn coolant on in toolpath programming.

7- Not setting the proper retract in in programming toolpath.

[Andre' B]

These seem to be my most common mistakes.

1- forgetting that top of stock is z= .75 not z=0 (hence drills and endmills crashing in to the part

Then why not always make the top of the part the Z zero?

2- clamps too close to the endmill path or tool holder

Dry run with the tool just above the part using single step with one hand always on the feed hold override, you should be able to read the line of code that is to be run next and know what should happen next. Keep an eye on the distance to go numbers, if they say the tool is going someplace it should not then stop it. Also should have the rapid override turned down to no more then 25%, depends some what on how fast your machines rapids are and how fast your reflexes.

Works for shorter programs does not work so good for CAM generated programs but then that is why you should not be using CAM until you can read and write G code.

3- smacking drills into parts while setting up parts

Don't do that.

4- forgetting to turn spindle on when resuming an operation that was terminated with emergency stop (tool crashes into part)

How does that work?
On every machine I have run hitting the E stop results in having to power down and reboot to reset the servo drives.

5- Rapid moving mill table in wrong direction crashing into servo casing (forgetting the right direction) this is a problem with the long frame parts where there is no room for error like that while setting up.

6- Forgetting to turn coolant on in toolpath programming.

Don't do that.

7- Not setting the proper retract in in programming toolpath.

Again if the work offset Z zero is always the top of the part then G0 Z0.1 gets you to a safe height to move around in X and Y.

Standardize the format of your programs so thinks just get to be a reflex.

Something like below.
First some comments about what the program does, also the name of the file it is stored in off line and which program it is of how many programs in that file. In case there are subs.

Next some safe lines that put the machine into a know state.

Then the tool change, note the M1 before and after so you can op stop when needed, say tool 1 is running but you know that tool 2 needs the inserts indexed, just turn on the op stop and it will be waiting when tool 1 is done.

Then set the work offset, get spindle turning, and put on tool length offset while dropping to 1 inch above the part and turning on the coolant. Then the rapid to Z0.1 before starting cutting, this move give you a chance to eyeball things after making an edit to at tool length offset (which anytime to do you should single block up to this point just to be sure you did not shorten the tool by 5" instead of 0.005"). This sequence should always be the same, but for taps which do not get the spindle turned on, the G84 takes care of that. You get so used to it that if anything is not right you just stop the machine and then figure out why you did.

%
O1000(8836-CHAMFER-KEYWAYS)
(MILL CHAMFER ON KEYWAYS)
(DSMV0035-1/1)
()
(ZERO IN CENTER OF PART)
(TOOL LENGTH FROM V-POINT)
(OF 90 DEG. TOOL)
(ABOUT 0.019 FROM END)
(OF A CHAMFER HOG)
()
G0G17G20G40G49G80G90
G91G28Z0M5
G69(TURN OFF ROTATION)
()

N1M1(FIRST TOOL)
T1M6
M1
G0G90G58X0.000Y0.000
S6000M3
G43Z1.000H1M8
G0X0.2143Y0.5775
G0Z0.100
G1Z-0.088F50.0
G01 X0.0690 Y0.7228 F10.00
G01 X0.0690 Y0.8275
G03 X0.0440 Y0.8525 I-0.0250 J0.0000

(do stuff)

G01 X0.5775 Y0.2143
G0Z1.000
G91G28Z0M5
()

N2M1(SECOND TOOL)
T2M6
M1
G0G90G58X0.000Y0.000

(etc.)

G0Z1.000
()

G91G28Z0M5
G91G28Y0
M30
%

[Geof]

After two months you should not be just 'forgetting' this and that. Think of a comparison; do you occasionally 'forget' to give way at intersections while driving? This can be risky if a Semi is barreling down the cross road and has right-of-way. You need to adopt some better work habits and develop a mental checklist before you forget you way into having a fragment of tool bury itself in your eye.

[Rich05]

After two months you should not be just 'forgetting' this and that. Think of a comparison; do you occasionally 'forget' to give way at intersections while driving? This can be risky if a Semi is barreling down the cross road and has right-of-way. You need to adopt some better work habits and develop a mental checklist before you forget you way into having a fragment of tool bury itself in your eye.

I have been told everyone breaks some tools first few months. But seems from these posts that its not that ordinary. So well that bodes badely humph.. Just keeping fingers crossed can start eliminating these mistakes. One factor for me is pushing to hard working on the stuff too long getting tired for sure. Other is just having to learn stuff the hard way... often.

[Mitsui Seiki]

What ever you do,don't rush things.Use "single block" if you're unsure what the machine will do and keep your hand on the "feed hold" button ready to stop it.

[under-dog]

What ever you do,don't rush things.Use "single block" if you're unsure what the machine will do and keep your hand on the "feed hold" button ready to stop it.

Agreed take your time. I still have mess ups but minor. I always watch carefully when things start to make sure I have everything going the way I expected. Most of your mistakes sound like rushing and hard to do if you are watching carefully. I have never crashed into motor stops even on my small taig. Keep your hands on stop and watch carefully. It should take more than a few moments to move that distance and crash.


I always make the top of the part "0" as well.

[Eurisko]

Rich,

These crashes bothered you enough to make a list of your mistakes and post it for all of CncZone to see.

Good news. There is hope for you.

My advice is:
Don't rush.
Don't allow anything to distract you from your work.
Double check everything.

As the man said,
First you get good, then you get fast.

As for me, I'm a perfectionist.
Good isn't good enough, and fast isn't fast enough.

[M0NKEY2TO2]

You cant be a machinest without scrapped parts here, and broken tools there. My first few months in my newest job I scrapped a $600 z setter, $300 octamill, countless collet holders and collets, over 100 E/Ms and drills, and alot of parts. This was just in my first few months. Now my numbers are down, but you gotta realize that there are hundreds or thousands of characters in programs. A zero here or a decimal there can be the difference from .05" and 5" deep. Proof slowly at slow rapids, dont use live parts (make a test piece out of aluminium), and always double or tripple check everything you do. Remember that 300ipm is a blink of an eye away from a trashed part.

[ImanCarrot]

Also, never machine when tired, it's just to easy to jog in the wrong direction, fast feed the tool into the part in Z instead of jog etc etc.

As said previously, dry run everything (blobk by block if you can) and cut air for the first run to make sure the tool goes where it should. Again I agree with the feedrate overide comment- get ready to rack it down to 0% or have your hand over the E-Stop.

The fact that you're addressing the problems is good. Good luck!

[CarbideBob]

I've trained about 60 people on cnc machines and I'd say you're not doing too bad.

I draw arrows on the table showing the axis jog directions with a felt marker.

If I'm not sure of a program I sometimes offset my program (G92) so that it runs and inch or 2 above the part for tryout.

Feedrate and Rapid overrides at 10 percent give you lots more time to hit the stop button if something goes wrong.

Don't feel bad. Buddy of mine with over 15 years experience ran his linear motor gantry machine into the side of a mold at 2500 IPM. Tore the entire 4th and 5th axis milling head off the machine. Total bill $64,000.00

The best way not to make mistakes is through experience. The only way to get experience is by making mistakes. All I ask of my guys is that every oops teaches them something. (of course it's hard not to get mad when I'm the one footing the bill)
Bob

[JDenyer232]

Aways verify your program and offsets using single block and low rapids to make the first part, once the program and setup is proven you can let her rip. Develop work habits so that you always do things in the same order. For example I always load my tooling first, set my work coordinates second, and set my tool length offsets third, I'm less likely to forget something if I always do it in a certain order. Also when using single block and low rapids be sure to check your distance to go display, if you know your endmill is supposed to go to -.250 and you see the distance to go showing -2.5, you know you are gonna crash. Here is a link to an article that may be of some help to you.

http://www.mmsonline.com/articles/cnc9810.html

[Chincia]

I am an agressive amateur. I have broken about 10 tools in the first year. Have done the following to reduce it:

1. I document the program like Andre said. I even put the definitions of odd G & M codes in a short table in the program.

2. I copy the tool offsets into the program so I can see them when modifying and running the program.

3. I cut a part 2 inches above the plane first.

4. I bought sheets of foam, glued them together to approximate the size of the beginning stock, and make a part in foam. When ou screw something up this way, you get a flurry of foam pieces as you are scrambling for the pause button.

5. I always make Z=0 at the surface.

[Rich05]

Thanks for the advise. I have been reading up where possible. Will study over these links as well.

[chunkymonkey]

Single Block And Feed Rate Overide Are On Machines For Reasons. Take Your Time, Take Some Notes, And Ask Some Questions. Observe The Best Guy In The Shop. Do What He Does.

[JROM]

Your getting a lot of good advice, but I'll just add my two cents.
ALWAYS set Z 0 at the highest point on your part.
Then set your R plane (retract) some distance above Z 0 and do ALL your rapid moves at or above the R plane. This is in stone!
The idea about drawing on the table with a magic marker is a good one, I still do that after 25 years running these beasts! And last but not least is my favorite saying about CNC machines
THEY ARE SMART ENOUGH TO DO ANYTHING YOU TELL THEM TO DO AND DUMB ENOUGH TO DO IT!!!!

[cadfish]

Another thing is to always remember to put the right tool in and double check that it is the right tool before pushing the green button. I didn't do that once luckily I didn't ruin the spindle bearings, and had a nice supervisor. I also was working next to a guy that some one told him to push the reset buton after every run once he forgot and then remembered mid-run "reset." Its interesting how a $500, 1 inch threadmill broke along with the thin walled aluminum cast part, the guy then walked off and was fired for not staying. So if You mess up stay and work things out.

[Switcher]

The 2 things I use most (all new programs), have already been posted:

1) Single Block

2) Feed Rate Overide




.

[Chris64]

I've been CNCing about the same amount of time as you. I've definitely had to hit the panic button a few times. I've been using 1/2" end mills so they don't tend to break as easily - but I have had a few servo overloads jamming the tool. I have chipped the corners on a few of them...some I have no idea how it happened.

I blame most of it on my controller (weak excuse, I know). It is riddled with booby traps. Ultimately they all could have been resolved by taking my time, checking things twice and always do a test run above the material.

Now, back to my controller...Every time a program runs, it automatically switches back to incremental mode, so moving doesn't always do what I expect. Also, programs uploaded get screwed up sometimes (again, testing would resolve this) but arcs entered like this X10.Y10./X0./Y10. will crash for no reason on the XY...but the /X/Y will work so out of nowhere I get a random rapid move in a direction I wasn't expecting (what should be the center of the arc).

That said, it also taught me how fast my machine can cut! I was running a 2 flute 1/2" mill through 3/8" 6061t in a single pass and did a quick 1/2" rapid right through the middle of it (~4000 RPM). It actually cut it OK (that's at over 100 IPM). I was probably very lucky it was such a short jump that "things" were able to deflect enough to keep it from blowing up on me.

That was my lesson about not testing every program above it first.


Now when I was trying to drill holes with a .040" drill - well that's another story...I had at least 30 casualties in that one.

[pdaly]

I,ve been maching on a Bridgeport VMC 600 with fourth axis for nearly 8 years now
Never crashed it !
My approch is very simple any time i write a new program i stand there and watch it with hand on the feed controll
If its a very long program i listen for tool changes-then race out to the machine and throttle back the feed untill i confirm the new tool is doing what it should be doing! And of course keep a record of programs that you've proven (Once proven let it rip!)
And just to make you feel better... when i first started learning CNC i buried the head of an old Deckel Maho into the table at full wack!!! ouch!

Have fun
Paul

[ImanCarrot]

Just to make you feel better

I rammed 800 quids worth of diamond tooling into a Germanium Dome which the raw material alone cost 8 grand. I thought I was in Jog mode, but was actualy in rapid Z move. It exploded like a grenade wrecking the component, the cutting tool and the glass vacuum chuck (another 2K).

Thank god I had impact shields up.