To the dark side CNC

[jadge]

I've never used soft limits; not sure I really see the need? One of the features of the backplotting software I use is that it gives maximum excursions in the three axes. So it is fairly simple to check the limits against the size of the part. This is especially useful in Z to ensure that the tool isn't going to get driven into the table.

Apart from the normal self-induced finger trouble foul ups I've had a few issues with my machine over the years. There have been a couple of electrical problems, both intermittent, one a dry joint and the second due to a poor quality copy of an industrial connector. I have had one Mach3 issue. Infrequently the tool would go racing off into the middle distance, milling through everything in the way. I eventually twigged that it only did it after a tool change. Turns out that somehow the tool change macro was changing to relative coordinates. I modified the post-processor to include setting absolute coordinates at each tool change. I also dumped the ordinary PC, running a clean install of XP, and changed to a controller running an embedded version of Windows. I haven't had any problems since.

Here are a few random thoughts:

I use mostly 2, 3 and 4 flute centre cutting end mills, and have standardised on 6mm and 10mm, unless I need a specific (normally smaller) size

Although my CNC mill and the Bridgeport are nominally the same hp, the CNC spindle is much faster, so I tend to program with smaller cutters running at higher spindle speeds and feedrates than on the Bridgeport. My CNC mill has a sort of 'quick change' collet system, which I have also started using on the Bridgeport for many of the smaller cutters

Almost all cuts are started by ramping down, or following a helix, to the required depth at about a third of the normal feedrate

I try and use as big a depth of cut as I can - you're paying for the cutting edges on the flutes of the cutter so you might as well use them

When cutting internal radii I use a cutter that is smaller than the radius; otherwise the angle of engagement changes rapidly and is almost certain to cause the tool to chatter

I use flood coolant on everything except, brass, cast iron and plastics, mostly to wash away the swarf rather than actually cool anything

'Touching off' carbide tools is a PITA. I chipped so many cutters I invested in an electronic tool height setter that automatically fills in the tool table

Andrew

[Stuart]

Thanks for the info Andrew

As is normal in engineering in general there are many ways to achieve the same result

Still getting to grips with things as has been said its a steep learning curve


Although my machines are much smaller than yours I do not nibble with cutters and like you I will use a smaller cutter to enable more flute to engage with the HP I have


Stuart

[kvom]

For touching off I use a 1" gauge block, and have never chipped a tool.  I jog up until the block slides underneath, the down .01" and then up by .001".

I use air blast to clear chips.  Tried coolant, and it was messy.

[maury]

I have just tuned into this interesting thread. Lots of good info. It demonstrates what was said in one of the early responses, every CNC user is on his own to build is system within his constraints and to solve his own problems.
Good stuff.

KVOM, I don't want to hijack the thread, but this might be relavant. Your response on "touching Off" intregued me. I have been dealing with backlash issues on my machine and for many reasons I don't want to go through the process of rebuilding. For setting the "Z" I have been using my Reference tool, dropping down to near the top of the work, and stepping down .0005 per step, using a .005 feeler guage  to touch against. Then step down .005. This has not been very reliable.
Question: do you believe if I step up like you do my "Z" settings will be better?

maury

[Hugh Currin]

For touching off I use a 1" gauge block, and have never chipped a tool.  I jog up until the block slides underneath, the down .01" and then up by .001".

I use air blast to clear chips.  Tried coolant, and it was messy.

I do the same. However, you need to be careful lowering the tool onto a block (i.e. don't do it). if asked to move say 0.010" down the machine will use all its capacity and force to complete the move. There is no "feel" in lowering the spindle. I typically move the tool a little below my 1" block. Then move up by 0.010" steps till the block slides under the tool. Then lower the spindle by 0.001" steps. Remove block from under tool, lower spindle, slide block under tool. Continue until block won't won't slide under and set tool length. It goes quickly and sets the Z axis to take up backlash on lowering moves.

I've had good luck with mist coolant. It's a little messy but not nearly as bad as floor coolant.

Thanks.

Hugh

[maury]

Hugh, the way I understand what you wrote is the tool is lowered until it touches, ( the way I do it). I understand the  way KVOM does it, he raises the tool until it just touches. The difference is which way the backlash is taken up. On Most CNC systems this is not an issue, but I'm finding it is on mine.

maury

[Hugh Currin]

Hugh, the way I understand what you wrote is the tool is lowered until it touches, ( the way I do it). I understand the  way KVOM does it, he raises the tool until it just touches. The difference is which way the backlash is taken up. On Most CNC systems this is not an issue, but I'm finding it is on mine.

maury

Maury:

Yes, I agree on the backlash. Using LinuxCNC I have the few thousands backlash accounted for, but it's still best (I think) to take up the backlash on a lowering move. However I don't lower the spindle onto the block when moving down. I move the block to the side, lower the spindle, then try to slide the block under the tool. So my process is:

1. Move the tool down (not over block) until block won't slide under the tool (visual no increment)
2. Move tool up by 0.010" steps till the 1.000" block slides under the tool
3. Move block to the side away from tool
4. Lower tool by 0.001"
5. Slide block under tool
6. If the block slides under the tool repeat 3, 4 & 5  -  If it doesn't slide under continue to step 7
7. You're done, set length compensation and go on to next tool

The Z axis drive will use all its power to complete the move requested. If the block is in the way it'll put a lot of force on the block and tool. I like to avoid this.

If I'm using only one tool, I'll typically lower the tool within 1/4" or so of the work. Then raise the table by hand using a piece of paper for touch off. Much better feel moving the table by hand than using the Z drive. Obviously for a knee mill where one can move the table up and down.

Does this make sense? Much harder (and longer) to describe than to demonstrate.

Thanks.

Hugh

[maury]

Hugh, thanks, I understand what you are doing. I was just wanting advice on which direction the backlash should be zeroed to.

Most of the time I just ignore the backlash, but right now I am trying to make some +- .001 parts that have setups on all 4 sides. I know this is a challenge, and am finding I have to do the precision part on my Bridgeport.

maury

[kvom]

That's exactly how I do it Hugh and Maury.

If you have backlash in the Z axis I doubt it makes much difference how you set zero since the spindle is going to move up and down when machining.  However, if your cutting is all -Z movements, then after setting Z with the block you can try to move up a few thou, then down the same amount and see if the block still just slides under.

[Dave Otto]

Add me to the list guys; Hugh, kvom, I set my tools on my converted knee mill at home the same way. for the most part I use a .1" gage block and sometimes I also will use a .001" feeler gage.  The knee mill is really lacking in Z travel so a height setter for the most parts is out of the question.

At work I have a nice 2" tall tool setter with a LED indicator light. When you get right down to it you can turn the LED off and on with one click of the MPG set on tenths. It is nice to have a relatively tight machine.

For cooling and chip removal I have a dual nozzle Micro-Drop system that I love. it uses a very expensive cutting lube/oil that is delivered to the tip under pressure at a metered rate. there is a second line that supplies air that carries the drops of oil from the tip to the cutter and part. The air and liquid are independently adjustable. It does not go rancid, smell, or fog up the shop. One gallon of the lube will last me many years. I have a solenoid wired into my CNC controller so the Micro-Drop is controlled by the the G-code.

I know a lot of guys get by with out limit switches and soft limits; but a good set of quality limit switches and properly configured soft limits sure are nice. My switches (Omron) repeat to a thuo or less; so if something happens and I need to restart Mach or the PC after homing I can go back to work with out having to re-do my G54 fixture offset. Also I can rapid full speed into the machine limit switch and when it gets to the safe distance it slows down at a controlled rate until just before it hits the limit switch and stops with out hitting it.

There has been more than a few times when soft limits have prevented a crash from a tool offset that didn't get set right.

I have servos on my mill and they move at a pretty good clip +120ipm. it is nice the have the machine not crash in to the the hard stops especially in the very short Z axis.

Just some of my thoughts,
Dave

[Stuart]

Dave
That's my thought on soft limits , but as a very raw beginner to the world of hands off machine I am posting my findings as first time user , I am just starting to crawl ( to use our own development in life)
Not looking forwards to the terrible teens when the think they know it all .

John MBE is coming next week for some hands on


Stuart

[Floating around]

Hi Stuart,

Glad I could help!

H.

[jadge]

Agreed that CNC can be a very steep learning curve, and I still have a huge amount to learn. It annoys me when 'experts' say it is cheating, as all you need to do is press a button and out pops a part. I usually tell them that since it is so easy they can come and use my CNC mill, but if they damage it then they pay for a new one. No takers so far!

The only way to learn is to give things a go. It is surprising how complex a part can be using only 2½D operations. I made 8 of these heatsinks, using only 2½D operations, a couple of months after starting from zero with CAM and CNC milling (I was already reasonably proficient with 3D CAD):



The heatsink is about 300mm square, and was a challenge to jig as that is bigger than the Y-axis range on my CNC mill, so it had to be done in two bites. All the small holes are M4 - I use a compression/tension tapping head on the CNC mill.

Using 3D operations opens up a whole new world, like this bevel gear (it is a true bevel gear, not one of the normal approximations):



And for 4th axis anything goes, like a bevel pinion:



Or worms:



When machining the worms I had all sorts of issues with feedrates. Basically the radius compensation 'feature' in Mach3 is less use than a chocolate teapot. I ended up using inverse time feedrates, G93. Although the worms look complex the G-code was hand written. The basis of the program is one G01 move in X and A. After cutting keyways the worms look like this:



If I can make parts like this then I am sure everybody else can too. 

Andrew

[Stuart]

Andrew

I have gone a shade of green no I have eaten something that has upset me but the learning curve has just got a whole lot steeper can you go steeper than vertical ?


Just got my 4 th axis set up working so when I need it it's there , got to sort out some tooling plates

But things are slowly coming together just waiting for John MBE to sign off on the setup and things should be OK

Decided to jump ship on turbocad for Mac and go down the Fusion 360 route , it's free works on the in house macs so I can do the CAD/CAM in comfort

Thanks again for your input
This must be the longest I have had a new machine and not cut metal

Stuart

[cfellows]

Stuart, you are going to love the 4th axis.  Since building my 4th axis, I've used it to make spur gears.  I also made a right angle drive for the spindle so I can use the 4th axis to make helical gears and do very nice and accurate threading.





<a href="https://www.youtube.com/watch?v=6HO0DICwnSk" target="_blank">http://www.youtube.com/watch?v=6HO0DICwnSk</a>

Chuck