How do you align precisely when you have to flip the plate over and cut from both over- and underside of plate ? My experience is that it easily gets 1-2 mm. misaligned.
1 Like
Hi @OSLO,
A typical trick is milling two reference holes somewhere in the stock on the front side (in an unused area not impacting the final piece), all the way through and down into the wasteboard. Then, flip the piece and use dowel pins (the same size as the holes) to reposition the stock for the back side operation. This will guarantee that the front and back sides are aligned. You need to position the reference holes in the design such that they are symmetrical with respect to the flip axis.
I don’t have a great tutorial on hand, but look on the forum for “dowel pin” and you’ll likely find examples (and I’m sure others will provide links and tips)
2 Likes
I guess it should perferable be 4 cornering holes and then don’t reprobe (except z) ?
Yes, exactly, Z only (and sometimes that is not even necessary)
1 Like
The key thing here is to be able to flip your stock precisely along an axis that’s precisely parallel with your machine’s axis.
One way to do it is what Julien said: bore some holes through your stock and into the wasteboard and put dowel pins in them. If the holes are precise and the dowel pins are precise, you’ll know that when you flip your stock, those holes will be flipped precisely.
If you don’t have or want a wasteboard, you can either make a fixture instead or you can use my personal favourite: Saunders Machine Works fixture plates and their fixturing pins. The pins precisely reference against the holes in the plate, so you know that no matter where you put them, they’ll be square.
Either of these ways, the precision of your flip will be limited by the position of your holes and the fit between the holes and the pins, so make sure you do all you can to get them right. In particular, don’t drill holes but bore them with an endmill (or pre-drill, then finish with a bore operation). I’d recommend boring at a few different diameters to get the fit between pin and hole just right. You want it tight enough that there’s zero play when you try to move the pin. If you can, use a reamer to get super tight tolerances.
The super nice thing about this approach is that if you set up your operations to be relative to where the pins are, you don’t have to re-zero the machine at all, you keep the same WCS for both operations.
An alternative to pins is milling a reference edge or two. If you mill an edge attached to your machine bed (e.g. an edge of some waste stock you bolted down) and mill an edge on your workpiece, you can precisely align the two edges, so you can precisely flip the stock knowing it’s aligned. You’ll need to figure out how to zero the stock on the axis perpendicular to the milled edge though.
1 Like
I decided to add 4 2mm holes in the corners in the front cutout. After cutout I will hammer 4 small nails in and cut the head of.
Is there a trick to get z right without actually probing z after changing drill ?
That’s what the BitSetter is for — is that not working?
Sorry, I had never heard of BitSetter. How does it work, since you are inserting a new drill of varying length manually ?
It’s an accessory for managing tool length offset:
Trick? No. (But there are many places where not following proper procedures will make a badly mismatched part). Want to make better parts…read on…
Trick no…Method(s)…yes (please read this more than once…maybe even print it out for reference)
The CNC needs to know where the X0, Y0 and Z0 are (this you know) but as a master of multi-sided machining (almost a daily thing for me), you need to prep the material so that when it’s flipped, and reset the XYZ. they need to be (either) in/or from the exact same location, OR exactly referenced to the original XYZ location.
Additionally, most material will move as the material is removed (stress reduction) and this also needs to be taken into account.
Prep your stock. It should be square (all four sided (or at least 2 of them and marked which one are square) and the flat. I cannot stress how important this is. If you look at the Carbide3D Flip Jig, it used the precision machined aluminum to remove the variability of the stock.
There are several ways to perform perfect double-sided machining.
- X and Y off two adjacent sides (that have been prepared and are 90º (not 89º or 91º) apart.
- Drilling a small hole in a board (in a location that can be removed at the last step) for the X0,Y0. For wood, I like to make this hole the same size as my cutter and (carefully) lower the cutter into this reference hole to reset the X0, Y0 when you flip the part.
- Using a milled feature of the part as a second place to relocate the X0, Y0. (Example, if the part had a large circular hole in the middle)
- Additional more difficult methods happen after you master the easy ones (mentioned above).
But what about the Z Richard…well, I’m glad you asked. Since wood is almost NEVER flat AND/OR parallel, flipping the material will often give you a Z that is a little different from the first (warping, non-flat, not parallel enough), and when machining multi-sided, a little deference in Z is a LOT OF ERROR. So I treat my Z height a little differently than most people…and my way is easier and (always works produces a perfect part) So here it goes…it might sound a little complex, but it really isn’t, and it gets easier the more you use it.
Setting the Z for Multi-Sided machining:
Step 1: Set your Z from your material (As Normal).
Step 2: Mark a location on your table (I use Front Center) with a marker/tape outline/etc). Move the machine (spindle) to this marked location and press the Z+6mm Preset location, then type into the MDI tab, G0Z0 (this will lover the machine/cutter to your Z0.)
(Choice 1) Make a block that is the same thickness as the distance from the bottom of the cutter to the table, in this location, the block thickness might be a little different, depending on your machine. (e.g. 3/4" (19mm) is a common size for most woodworkers) Mark the wood, and SAVE it as a Z Set Tool and its thickness.
Choice 2) (My method) Purchase a set of Grade B Gauge (Gage/Joe) Blocks. ($80 Amazon) Make up some blocks that are the same thickness (distance) as from the bottom of the cutter to the marked spot on your table. (I use masking tape to hold the blocks together (placed on the side of the blocks…NOT the top/bottom)
Step 3: Flip your material set your X0 and Y0 from the same edges as the First side machining. You may or may not need to reset your Z if you are only using one tool. But if you are using multiple tools, Move the machine to the preset location and lower the Z (carefully) onto the Block (from above Choice 1 or 2) and reset your Z using the paper method.
I LOVE my BitZero…for normal machining…but I NEVER use it to reset my Z when making multi-sided parts. The BitSetter should also work too, but if you don’t have one, these instructions will help you.
EDIT ADD: BitSetter Concerns, It will want a NEW Z0 when you load a new program (eg 2nd side program), BUT the new Z should be the same as program one (1st side), so be careful WHERE you set the reference Z for the 2nd/3rd/4th side etc. (not a problem if you use my method, you just need to remember).
Can you use it (BitZero) for resetting the X0 and Y0, YES…but remember if you started it in the Lower Left (which Carbide3D Probe macro uses) and you FLIP your material for the second side…it will NOT be in the Lower Left position now…what was on the left, is NOW on the right…etc.
PS The CNC program for the second side, needs to be referenced from the new flopped XYZ location. Assuming you know that…yeah I know.
Once you do this a few times, it becomes second nature, and easy. Making double-sided parts (or 4-sided Chippendale Ball and Claw desk legs…look them up) is the next step in mastering your CNC…and makes a part much more valuable…$$$$
Question? Ask away…if they are really silly…PM me…it’ll be our secret.
6 Likes
Another option is to keep the “J” corner in the same place. This involves making sure one corner of the stock is nearly perfectly 90°. Then rather than flip horizontally (around Y) or vertically (around X), flip the part around a 45° imaginary axis from bottom/left to top/right. Or just mark the “J” corner (usually lower left), flip the part & turn it so the same corner is at the lower left.
I like using fences, and make it a habit to make my zero point always lower left corner on the bottom of the part, or top of table. This results in all your numbers in the G-Code being positive numbers, in the 1st quadrant of cartesian space.
Of course, this only works when the job will fit on the machine when flipped this way, and the “J” corner remains after cutting the 1st side.
So it’s good to know several different ways of setting up parts and choosing the best method for that particular job.
2 Likes
This topic was automatically closed after 30 days. New replies are no longer allowed.