Probe a cylinder

1

Forgive me if I couldn’t find where this was asked and answered before, but is there a best practice someone has come up with for setting the zero for an operation at the center of the end face of an existing cylinder of stock material?

image
image1125×915 48.9 KB

Thanks,
Adam

1 Like
2

How precise do you need to be?

You could use a center finder like one used for mounting material in a lathe, and then just eyeball it:

If you are sure the material is circular enough for your purposes, you could measure the diameter, then use an ‘L’ fence. Probe the corner using a block, then you can set the zero based on the radius. A trick for this would be to zero out at the corner of the ‘L’, then go to the ‘Set Zero screen’, and enter the negative of the radius as the X and Y co-ordinates. Now move to zero, and you are over the center of the cylinder.

1 Like
3

Nice on setting the negative for an offset. The only issue with an L block is aligning the sides of the L with X and Y since I have to flip the cylinder and do both sides.

Thanks,
Adam

4

Mount a spoil board, cut a circular recess ‘on centre’ for your zero, then mount/hold your stock in the recess - knowing it is centred. Flipping will be interesting unless rotational alignment doesn’t matter - scribing a vertical line down the side of your stock and making a matching mark on the spoil board could be one way (visual alignment).

3 Likes
5

Use the machine to machine a square L? Tack down some scrap MDF, machine an L into it, boom it’s automatically aligned with your machine. Set your Zero as the corner of the L that you machine and you don’t even have to probe to get that location. Since it’s a cylinder you don’t even have to care about clearing the corner, the cylinder won’t be anywhere near it.

2 Likes
6

If it’s a metal cylinder you can go old school to find the center.

Assuming you have a router and not a spindle (and thus can’t just run an edge finder).

  1. Put your bitzero on top of the stock so that the stock is electrically connected to the bitzero
  2. Put the router bit or preferably dowel pin you normally use with the bitsetter in the router and connect the crocodile clip.
  3. Using manual jog move toward the left edge of the stock and jog down in Z until the bit / pin will hit the side of the stock if you keep jogging, at about the West compass point, jog in at 0.025mm (smallest jog) until your bitzero light changes colour, set X=0 in the Carbide Motion app
  4. Now move round to the East compass point and jog left in 0.025mm increments until the bitzero light changes colour, read off your X co-ordinate.
  5. Jog up in Z to clear the workpiece and bitzero
  6. Use a calculator to divide your X position by 2 (e.g. if you are at X=121.2mm then 60.6mm)
  7. In the MDI move the machine to the halfway X value, something of the type G01 X60.6 F100.0 (Please do check my GCode, I’m rusty)
  8. Set X=0 in the Carbide Motion app, you are now centered in X
  9. Jog to the South compass point, jog Z back down, creep Y+ at 0.025mm / step until bitzero LED changes, set Y=0
  10. Jog to North, creep in, bitzero LED changes colour, read off the Y, let’s assume it was 124.8mm (you weren’t perfectly on Y=0 when you set X)
  11. Jog up in Z, move G01 Y62.4 F100.0, now set Y=0

That’s approximately what I’d do with an edge finder in my spindle.

2 Likes
7

That is pretty much how I do it - except I use an edge finder. Worth noting here it also has a dependency on the stock being actually round. I typically take a few thousand off the outside of the round stock with the CNC just to be sure what comes out is as round and concentric as the CNC can make it.

2 Likes
8

For folks who are concerned about symmetry and consistency between the two axes, please see:

9

@liamn @philg Thanks for the tips. Used some of both ideas. I held the touch probe to the side of the part since the cylinder is only 1.25" diameter and tall compared to z carriage clearance. Used the MDI interface with /G91Xxx or /G91Yyy to move to the center location.

I did have a bit setter zeroing issue for some reason. Plunged too deep and plowed into stock. Had to face all of that off of the surface. Bit setter has been working fine. I wonder if it was due to swapping mm to inches in the interface during the process? When running the program, it asked for the tool to be put in (already installed) then went and probed height, then came back and moved up and the Z axis ran into the top of the range and skipped steps, and then it plunged too deep. Clearly Z was confused for some reason, but I rehomed or reinitialized machine and ran it again and it worked.

3 Likes
10

Glad to hear you found something that worked, the more I work with the CNC the more I realise that it’s all about workholding, probing and measuring.

If the Z error was from switching units, you’re in excellent company.

1 Like
11

@LiamN I’ve heard the mars probe story. I’m more suspicious the z-error was Carbide motion bug, that toggling mm to inches in the interface somehow messes with the homing, but that’s speculation. It’s behaved reasonably well for me otherwise once I realized that the touch probe and alligator clip touching is what was causing the bit setter cycle to fail and now keep them purposely apart after use. The unusual plunge depth on an unpredictable basis appears to happen to others, too (Z-height issue with bitsetter - #11 by WillAdams), so I just kept my hand by the e-stop just in case after that.

Also, I second the idea that machining seems to be about measuring, workholding, and probing – that’s just not what you see in the advertising.

1 Like
12

Ah, sorry, wasn’t suggesting user error, more that switching between units, in software or wetware was a well known source of unpredictable behaviour. Switching units mid-task is probably not a set of test cases I’d have in my software test coverage.

13

This topic was automatically closed after 30 days. New replies are no longer allowed.