English Wheel Rollers and primer on CNC.

I’ve spent the last couple of weeks at Tafe working on the lower rollers for the english wheel. Since nobody was using the CNC machine, I decided to try using that to make the rollers. This turned out to be a big mistake, but a good learning experience.

This slideshow requires JavaScript.

The first thing to do is write the G-code. It’s a simple language that can be generated from toolpaths by software like SurfCAM, MasterCAM, etc, or it can be written manually for simple operations, which is what I did. The code is at the bottom of this blog, and commented.

The G code contains very basic instructions for the machine to perform, like turn the spindle on, turn the coolant on, move the tool from here to there, and so on. The machines don’t know kind of tool is in what tool post, or how big it is, what shape it is- you have to tell it. In order to make the machines as versatile as possible, there is very little in the way of safety overrides, making it quite possible for a careless operator to the tool into the chuck or drill a hole and then snap the bit by moving sideways without retracting first.

So, one the code is written, one needs to put the appropriate tools in the tool holders and then input the tool offsets into the machine. The CNC machine knows where some reference point on the tool holder is, but not where the actual cutting tip of the tool is, so it’s standard practise to carefully move the tool in and take a bee’s-dick-sized cut off the face, at which point you can measure the workpiece and set the tool’s Z direction offset as the difference between what the piece measured to, versus what the machine’s spindle position was. So for example, you do a cut at say, 52mm and measure the workpiece. It turns out to be 54.53, so your tool offset is whatever the old tool offset was, minus 2.53. There’s usually a calculator in the machine for that. Then if setting up a normal turning tool, you would take a skim off the outside and measure the diameter. You then change the X offset to compensate. I found out the hard way that you should DEFINITELY use the machine’s calculator for this, because you might not know whether the offset is radial or diametric, or positive or negative.

Incidentally, a lot of machines have a probe that you can use to set the tool offset. They’re pretty good and makes the last paragraph redundant.

This should hopefully get you fairly close, so now, depending on whether you’re turning rubbish or expensive material, you can just make a part and measure it afterwards, reset your offsets and keep refining. If you’re making parts from expensive material, you would want to check your offsets by doing a cut the same depth as your program’s finishing cut. Depending on how accurate you need to be, the finish cut’s radius, the material, presence of coolant, coolant temperature and the machine’s temperature could also have an affect. This is where it’s easy to get caught by having a perfect view of a very imperfect world. The CNC machine may well say that the tool is at 31.126mm, but the tool will easily deflect 0.01mm on any decent depth cut. Thermal expansion can also make 0.01mm difference in the workpiece’s dimension, as well as the position of the tool in the CNC machine due to differences in the expansion of all the parts of the machine, which is why a good operator warms a machine up before making anything of importance. When you’re making a part that’s measured in tenths, 0.00’s or cunthairs, you have to think a little bit harder.

Anyway. After setting up the tools and fucking around with tool offsets for a long time, I managed to rough out 6 rollers, but the bearing surface was undersized on all of them (I was having a looot of trouble with the tool offsets. Remember what I said about radial/diametric/positive/negative?). I ended up using a manual machine to finish them, as it generally takes an hour or two to set up the tools and offsets. Generally, in a workshop, you only need to do this once, but at Tafe, the tools get moved around and you can’t trust previous operators.

The tool post.

In order to machine them on a manual machine, I put the rollers in a 4-jaw chuck and clocked them up with a dial gauge. I measured the bearing bores with a telescopic bore gauge and micrometer, as there weren’t any bore micrometers.

The trick to using these is to put them in the bore at an angle, rock them around a little bit to ensure they’re at the centre of the bore, tighten them at the base and then pull them out while rocking them through the centre. According to the yarchive, they’ll read about 0.01mm too small. I’ve found that I can get a repeatable measurement that’s consistent to within 0.01, but it does take some practice. I usually measure 3 times to make sure.

Put in on angle, rock around, nip up, move through centre line.

OK, that’s enough writing for now. G-code below. Enjoy.

O5555                              ‘ This is just the program name. Different machines like different syntax in the first line.
G50 S2000                     ‘ G50 on this particular machine sets the maximum spindle speed, in this case to 2000 RPM. CNC Machines constantly vary the spindle speed so that as the surface speed is constant regardless of what diameter the tool is currently cutting. A maximum is set so that the machine doesn’t go to maximum RPM when you’re facing and the tool goes near the centre of the workpiece
G00 X500 Z500            ‘ G00 is rapid movement. This sends the tool to the home position.
T0101                              ‘ Select tool 1 with the tool 1 offset. The tool offset tells the machine where the tool is relative to the chuck so you can change tools around. You also use this to compensate for tool wear so you continue to cut accurate parts
G95 F0.1                         ‘ Set feed rate to 0.1mm per revolution
G96 S200 M42              ‘ Set surface speed to 200m/min in (I think) low range gear
M4                                   ‘ Spindle on in clockwise direction
G00 X70 Z10                 ‘ Rapid to X=70 and Z=10
M08                                 ‘ Coolant on
G01 Z4                            ‘ Feed in to z=4
G01 X-1                          ‘ Feed to X=-1. You go to -1 instead of zero because your tool will have a radius on it. You end up with a nib in the middle if you don’t compensate.

The cutter radius won’t be considered when facing, so you should machine from x=outside diameter to x=-1, rather than x=0, otherwise, you get a little nib in the centre of the workpiece.

G01 Z5                           ‘ All these lines are just moving the tool around to do the cutting. The blanks were all about 65mm in diameter and 52-54mm in height. I set the work offset to 1mm and cut them down to 50. This ensures that there’s a minimum of 1mm left to face the other side and also ensures that they’ll all get faced. The following lines will therefore cut the workpiece to diameter 50 and height 51.
G00 X70
G01 Z3
G01 X-1
G01 Z4
G00 X70
G01 Z2
G01 X-1
G01 Z3
G00 X70
G01 Z1
G01 X-1
G01 Z2
G00 X70
G01 Z0
G01 X-1
G01 Z1
G00 X65
G01 Z-26
G01 X66
G00 Z10
G00 X63
G01 Z-26
G01 X66
G00 Z10
G00 X61
G01 Z-26
G01 X66
G00 Z10
G00 X60.5
G01 Z-26
G01 X66
G00 Z10
G00 X60
G01 Z-26
G01 X66
G00 Z10
M05                               ‘ Stop the Spindle. This operation is done.
M09                               ‘ Coolant off
G00 X500 Z500          ‘ Rapid to home position. A common mistake is to do this from the end of the last cut, which, if in a drilling or boring operation could be inside the workpiece’s bore. So make sure you have the tool outside the piece before you do this!

T0707                            ‘ Select Tool 7 and that offset. This is a universal drill and so is used to drill out the centre and then to do some rough boring.

G95 F0.1                      ‘This is more of the same so I won’t comment much now. These movements drill and bore to diameter 30 on the inside.
G97 S600 M42
G00 X0 Z10
M03
M08
G01 Z-55
G00 Z10
G00 X5
G01 Z-55
G00 Z10
G00 X9
G01 Z-55
G00 Z10
M05
M09
G00 X500 Z500
T0303                                 ‘Now select tool 3 and finish bore the inside profile.
G95 F0.1
G96 S200 M42
G00 X30 Z10
M04
M08
G01 Z-21.5
G01 X29
G00 Z10
G00 X 32
G01 Z-21.5
G01 X31
G00 Z10
G00 X 34
G01 Z-21.5
G01 X33
G00 Z10
G00 X 34.5
G01 Z-21.5
G01 X34
G00 Z10
G00 X36.5
G01 Z-16.5
G01 X36
G00 Z10
G00 X36.98 Z10
G01 Z-16.6
G01 X35
G01 Z-21.6
G01 X28
G00 Z10
M05
M09
G00 X500 Z500
T0303
G95 F0.1
G96 S200 M42
G00 X30 Z10
M04
M08
G01 Z-21.5
G01 X29
G00 Z10
G00 X 32
G01 Z-21.5
G01 X31
G00 Z10
G00 X 34
G01 Z-21.5
G01 X33
G00 Z10
G00 X 34.5
G01 Z-21.5
G01 X34
G00 Z10
G00 X36.5
G01 Z-16.5
G01 X36
G00 Z10
G00 X36.98 Z10
G01 Z-16.6
G01 X35
G01 Z-21.6
G01 X28
G00 Z10
M05
M09
G00 X500 Z500
M02
%

Advertisements
This entry was posted in English Wheel and tagged , , , , . Bookmark the permalink.

2 Responses to English Wheel Rollers and primer on CNC.

  1. James Richards says:

    hi Jared, There’s a really nice machine down the back next to the materials racks that’s only used by the tafe guys, they might let you play on that as i doubt that is ever molested by the students. did you use a program to compile the G code or did you define all those interpolations yourself? i learnt the Gcode for the lathe last semester, but have been busy with the chassis manufacture since then and haven’t had a chance to smash out a part. really want to give it a go this semester.

    • Hyllest says:

      Hi Richo,

      I’ve seen that machine but haven’t thought to ask to use it.

      I wrote up the G-code manually, since the parts are very simple. I did the same for the first curved profile cut, too, but the machine didn’t seem to want to read canned cycles. I was getting visibly frustrated, so the instructor offered to write the code out without while I set up the tool offsets.

      Believe me when I say that there’s nothing pleasant about CNC machining. It’s super frustrating getting the machine to work with the right tool offsets and stressful as you try to get it all going before the end of the TAFE session. Then there’s a massive anticlimax as you spit out 10 parts in the last half hour and leave for the night, only to have someone else change the tools and fuck up all the offsets as soon as you’ve gone.

Leave a Reply

Fill in your details below or click an icon to log in:

WordPress.com Logo

You are commenting using your WordPress.com account. Log Out / Change )

Twitter picture

You are commenting using your Twitter account. Log Out / Change )

Facebook photo

You are commenting using your Facebook account. Log Out / Change )

Google+ photo

You are commenting using your Google+ account. Log Out / Change )

Connecting to %s