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.
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:
. 
