Some thoughts on CNC: Crashes that we all have to make

Nathan the Machinist

KnifeMaker / Machinist / Evil Genius
Moderator
Knifemaker / Craftsman / Service Provider
Joined
Feb 13, 2007
Messages
17,541
Knife making is becoming increasingly CNC oriented, particularly folders. This has a lot of folks feeling their way around in a new skill and there is a learning curve.

I've been through all of this and I've trained people who have been down this road and I was thinking about this today while out in my shop. One common theme I've found is that errors are common and costly and it seams like the only way people really learn is to make a mistake and learn some fear from it before their subconscious sub-systems kick in and they recognize that something might cause a problem before it actually does.

I've come to realize, when training a new machinist, that they need to be in control in order to learn, that mistakes are inevitable and it is best to supervise them in a way where the mistakes can happen, but the broken tools are small in order to preserve the machine tool.

But, knifemakers learning machining and CNC, alone in their shops, don't have someone looking over their shoulder preventing the catastrophic crash that ruins a mill or causes an injury. So I've compiled a list of the mandatory muck ups that everyone does so you can at least have the chance to mull it over. Perhaps, having thought about it in advance, you might reduce your learning curve and the related tuition...

This is my list of mistakes that every rookie makes and learns from:

tall work piece slips in vise, breaks endmill
executing a tool change over a tall work piece with long tooling such as a drill and having the tool (or a neighboring tool in the carousel) crash into your work during the tool change
retract plane in drill cycle too low, breaks drill in counter bore or similar
send wrong program
zero the work piece or tool incorrectly
load wrong tool
inadequate tool stick out and tool holder collides
parallel moves during machining and a drill exits the back side of the work piece and hits the parallel
facemill stalls the spindle
tool pulls down out of tool holder in a heavy cut
plastic or wood part pulls up out of the vise
hitting the work stop that you think is set safely to the side with a big ass face mill
tapping deeper than the hole is drilled
and if you're using a CAD/CAM system, cutting on the wrong side of a surface or trajectory (sending the cutter through the part, not the air beside the part)

You could write a book about this, but I'm going to try and talk about some of these. And if you're getting into this, stop and really think about how it might apply to your work flow.

1: Tall work piece slips in vise. What happens here is a tall work piece gets stuck up out of the vice and you're cutting on the end of it. Being CNC, you're climb milling. The nature of climb milling is it wants to pull the work piece into the cut. The longer your work piece, the more torque it can put on your work holding. If it's long enough, and the work piece is perhaps not perfectly square or otherwise not well retained the cut can pull the work into the cutting tool. When it does, your chip load might go up from .004 to .040 and break your cutter.

2: The Haas minimill is one of the most popular cnc mills that a maker might buy. They're cheap (around $35K), they fit under a 7' garage door, they're easy to use and have 1st rate motion control. But they only have 10" of Z travel. And it uses some of that travel to execute a tool change. The tool change height (and the carousel full of tooling) is down in the working envelope. So when using long tools like drills and reamers you have to learn to double check and if necessary move your work away from the ATC before executing a tool change.

3: Retract plane in drill cycle too low, breaks drill in counter bore or similar. This one got me the other day. I was countersinking holes in the bottom of counter bores. I remembered to change my retract plane in the CAM system, but I forgot to change the output so that tweak would occur in the mill itself. So when it retracted to rapid over to the next hole it was still buried in the work.

4: Send wrong program. This is easy to do. Double check the time stamp on the file before sending it so you're certain you sending the right file. And engage the gear between your ears when you press the green button, is that the cutter and RPM you're expecting. We get complicate over time, and this last double check has saved my ass a couple times.

5: Zero the work piece or tool incorrectly. Just go ahead and assume you have. When it's a new program and a freshly loaded cutter, pause the program just before the cutter reaches to work and look at the "distance to go" screen and make you don't have another 5" of rapid z move while you're hovering an inch above the work piece. This saves my ass with some regularity.

6: Inadequate tool stick out and tool holder collides. Every rookie does this. It surprising how frequently they hear a problem but don't know what it is. Or they can see the work is messed up, but don't know why. People get so wrapped up in looking at the cut they fail to look at the tool holder. Once bit they start using too much stick out.

7: Parallel moves during machining and a drill exits the back side of the work piece and hits the parallel. You need to tap your workpiece down into the vice so your parallels can't move. If in doubt I'll put a spring in there to hold the parallels against the jaws. Some holes are close to the edge and you need to allow for that.

8: Facemill stalls the spindle. You're a knifemaker facing the can off some Elmax (nastiest stuff most machinists ever deal with) on the tiniest little mill. Yeah, it may be a 7 1/2 HP industrial machine tool, but it doesn't make that much power down at 400 RPM. As the inserts dull and the steel work hardens the cutting forces go up, the RPM drops out of the power band and you stall the spindle. When the spindle bogs down on a big face mill and the table keeps feeding you can brinell your spindle bearings in a single muck up. If you're near 100% on the load meter pull some inserts out of the facemill and slow your feed rate accordingly or get a smaller facemill.

9: Tool pulls down out of tool holder in a heavy cut. Rookies never see this coming. Heavy cuts and inadequate tool clamping pulls the cutter down out of the tool holder, making the cut that much deeper and leading to trouble.

10: Plastic or wood part pulls up out of the vise. You can't clamp across soft materials like you can steel. And it's tempting to use the high helix cutters designed for aluminum because they cut so well. But the helix of the cutter can pull the work up out of the vise and then throw it at you. Sometimes in this situation you need to use router bits because they have a low helix. You can also super glue sand paper to your vise jaws to give them more grip.

11: Hitting the work stop that you think is set safely to the side with a big ass face mill. Again, you get so involved with your cutter and work piece that sometimes you forget to look at what else is on the table.

12: Tapping deeper than the hole is drilled. Obviously you can screw this up the old fashioned way, but you can also run into trouble tapping on a machine without rigid tapping and having the tap overshoot while the spindle reverses. Or using saved parameters for tapping and forgetting to update the thread pitch. If you tap a 10-24 hole with parameters for a 10-32 hole, it's going to overshoot the bottom.


These are some of the pitfalls a maker-turned-machinist needs to be on the lookout for.


Some other words of wisdom:

Never interrupt a tool change. If you do, go ahead and assume the machine has lost track of the spindle status and remove the tool manually. It only has to think the spindle is empty once and try to pick up a tool while there is a tool already in the spindle to ruin your day

When you clamp the work piece both it and the fixed jaw are going to distort a little. This is important when flipping to side two of a part. Go ahead and assume things will move a little and add .001 positive Y tweak. You might need more that than, but you'll seldom need less.

I like to add tweaks to the global offset (g52). (Fanuc, Haas will do this with a parameter change) I like adding this to global so the values in G54 are what I measured, and the tweak is easy to see.

Learn to start a program in the middle of the program. You can use the search function to find the tool you're on in the program and start the program from the top of that tool.

Standardize your tool length offset plane and compensate either in your programming or in your work offset. Touching off tools in the carousel again when changing to another part is retarded. Don't use feeler strips, use a lighting touch probe, they're faster, more accurate and more forgiving.

Use a torque wrench to set your vise. It takes the guess work out of the equation and leads to consistency. You'll know with experience, "this part needs 20 foot pounds" and your work is more accurate and less dented.

If you're driving a nice car and have a shitty bandsaw your priorities are out of whack.

I hope some of my experience is helpful to one of you guys starting out down this road. I'm sure I've missed something so I welcome your input.
 
Last edited:
Thanks Nathan for this lesson. I'm not a machinist....yet, but it's contributions like these that make BF the best knife site out there.
 
Nathan, Awesome post. Had to laugh. Many if not all at one point or another I've done. I now have gotten my son hired into the shop I'm working at and since he graduated HS this past spring he has decided to pursue a career in CNC so back in July he got brought up into the CNC dept from being a part time sweeper/cleanup kid. It's been interesting since he's as green as they come to watch him do many of these same mistakes that all machinist experience. I just sit back and chuckle.

Jay
 
That page is getting printed so i can put it on my wall when i finally sell enough knives to one day merit getting a CNC mill... just bought my first table top mill last fall and it's already paid itself off, and i firmly believe that if im going to make a semi production run with any accuracy and repeatability that the mill is MY only option... my grinding inaccuracy usually gets fixed by my sanding and filing accuracy, or as i like to tell customers "each one may be a little different due to the hand made nature of the product" IE: I mess things up and have to fix them so some grind heights and plunge lines are different on most of my knives. The Mill doesn't have the same grinding problems i do!

thanks for your outstanding post Nathan
 
Excellent advice to anyone getting into CNC. I have made many of the learning errors on your list, and I suspect that most guys will as they learn. I've even had some CNC experience with lasers and other CNC fabrication equipment before purchasing my CNC mill, and anyone that thinks such experience will make them less likely to make these mistakes is mistaken. You need to find the combination of techniques, and order of operations that works with your machine, and some of that will even change between two different mills, let alone different types of machines. Be consistent, really really consistent, to avoid the "what was I thinking" mistakes. Approaching a part, program, or problem the same way every time (unless you know your past attempt was a failure) gives you a way to more accurately gauge exactly what is going on because you have eliminated some of the variables that can have you chasing your tail.

Your eyes and ears are your best assets when it comes to learning to keep your machine and parts safe. Look at the part, listen to the sound of the spindle, listen to the cut.
Are things vibrating?
Is the sound smooth and consistent, or does it have a lope to the sound of the cut(if so, your cutter probably lost an edge and the others will go soon if you don't take action)?
Does the spindle slow down when it enters the cut?
Can I do my -Z feed off of the part, or do I need to ramp into a pocket?
What exactly is causing my bad surface finish? <--- Early on I spent long time learning the hard way that this can be caused by high speed, low feed cuts, even with flood coolant.

Be aware that if you ask 3 different machinists how they'd make something, you're likely to get 3 different answers. What machines they've used and have now, their preferences for particular types of work, and past experiences with similar parts will all shape their approach. I'm talking about something REALLY complicated, not hacking profiles out of a sheet for knives, to be honest the few knives I've chosen to mill vs other methods, the mill always loses to hand shaping 1, or paying for a laser or waterjet to cut 10. Even in 3V I can cut and profile a knife for $3 worth of abrasives and an hour of my time.

So the main value for me (besides the fact that I already had it before I ever thought about making my first knife) of having the CNC mill for knife making is for jigs and fixtures, and prototyping something I plan to make in volume in a hurry. This math may work out differently for others, I always consider that every hour I'm working has value and has to be factored into the cost, so I consider the CAD/CAM time, building fixtures, milling, tooling costs, etc when I look at whether to outsource the process to the jobshop I've been working at for the last 8 years. They're ISO certified, pricing is excellent (and I pay their going rates, in fact I've insisted on it whenever it's been something I plan to sell), lead times are reasonable, and I'm intimately aware of the level of quality that goes out their doors and I can sleep easy knowing they will deliver EXACTLY what I ask for. I'm a manufacturing engineer making knives, so my approach to knife making may be different than other people but that doesn't mean it's better, it's just the culmination of MY experiences and knowledge and the path I'm choosing.

Great thread Nathan.
 
Last edited:
Thank you Nathan! :)


Great post with fantastic information.

Thank you for taking the time to share this!!! :thumbup: :cool:
 
You've been a great help to my son, Kevin, who taught himself to program and operate our 3 axis CNC machines. He comes from a tech background but had no machining in his history. He took a lot of small steps without to many setbacks along the way and now can program and set up the machine for production runs as a matter of course. I am very proud of what he accomplished.
Thanks for this post and all the others that have been so helpful to us.

Fred & Kevin Rowe-----Bethel Ridge Forge-----
 
Nathan, a CNC mill is a long way off in my future, but it is in there. I don't even know enough to understand most of your warnings, but I still appreciate them very much. I will be saving this post for when I am getting started on my CNC milling education in earnest, and I really appreciate you contributions around here.

Regards--Don
 
Great post Nathan! Wish I had a list like this when I was in the rookie phase. I've made most of these mistakes, and I'm sure others that aren't on the list :o.

For us one of the things that saves our butts the most is doing a "sanity check" on the Z height before letting the program run. You mentioned a visual check which catches the obvious problems. We go one step further and take a quick measurement (with a good old tape measure) between "Z 0" and the tip of the tool; then we compare the measured value with the Z value on the screen. There are so many ways that Z height can get thrown off (depending on your mill, fixturing etc) that it has just become part of our routine.

-mike
 
Thanks for this post Nathan. I'm getting my first mill in the shop this next week... albiet it's a dinosaur, no CNC here, this was designed to be run on line shafting! But it does good accurate work currently where it's stationed but isn't large enough for the engine work the current owner is doing, so he got a big brown and sharpe to replace it.

mill.jpg


What are some of the basic tools that you would recommend purchasing to go with it once it's in my shop? I've got a decent milling vice from a bridgeport, an 8 inch X+Y rotary table, and no real tooling. For knife work what type of mill bits should I be getting for slot work? Would a dividing head be beneficial to have if I want to mill even grip grooves around take down handle parts?

I know I dont have to worry about tool changes and whatnot, but I will have to try to prevent any crashes from noob mistakes, or running the table off the end of the feed screw and whatnot, so this post will help me think about things before I go and do something BAD (tm)
 
Last edited:
A comment on number 3. of Nathans list. One option to avoid issues with your tool retract height (Rapid Plane) is to add G98 to your drilling canned cycle line. G98 returns your tool to the initial Z height that you have programmed before the start of the canned cycle. Here is an example in which there is a obstruction between the holes of a 1 inch elevated surface.

G17 G20 G40 G49 G80
T1 M6
G54 G90 G0 X2. Y0. S2292 M3
G43 H01 Z2. M8 (Initial Z height that the canned cycle will return to after each hole is drilled when using G98, set this to clear any part feature or surface)
G83 G98 Z-1. R.1 Q.1 F20. (Drilling canned cycle with full retract)
X0. Y2.
X-2. Y0.
G80 M5
G28 G49 G91 Z0. M9
G28 G91 X0. Y0.
M30

Also another tip to add to the list is to double check your decimals, one misplaced or omitted decimal point can make a huge difference in a coordinate and easily cause a crash.

If anyone needs it I'll try to explain more about coding later if I have the time, hope that helped.
 
Back
Top