X Axis consistently off with 2nd side operation

Software Carbide Motion
1

I have been working on a perfect two sided machining technique for quite some time now. I still haven’t found it… But this is what I have so far:

I finally have a system that works fairly well… I will explain that first so that there is some understanding of what I am doing, and then I will share my problem.

To machine my pieces, I run the first cuts, side A, usually on the aluminum threaded bed, This first operation finishes off the entire front side and leaving a thin peel at the bottom of the product.

I then switch out the bed to a slab of MDF and screw it down.

Once that is done, I create a file in Carbide Create for second side B operation.

First I put the dimensions of the project at 8”x8” and then set X&Y Zero at center.

I then import my piece into that file and place it anywhere on the bed. It doesn’t really matter where.

After that I select just the outline of the piece and create a pocket operation to cutout out about 5mm deep into the MDF.

Once that is done, I export the file, jump over to Carbide Motion and set my X&Y center at the center of the bed in the Carbide Motion software. I then set zero against the height of the MDF and run the operation.

Once that is done, I go back into Carbide Create, set the chamfers for the side B operation, and save the file. Note that I haven’t moved anything. As far as the file is concerned, everything is in the exact same position. The only thing that changed was no more pocket operation, and now there is a chamfer operation.

Now, with my product in place and ready for the second operation, I open up Jog on Carbide Motion and set X&Y again at the center of the table, and set my Z off the top of my product.

Here is where the issue arises… Almost always, I the chamfer will be off by about .25-.5mm to the right on the X axis. No matter what I do or how many times I center everything again, it still happens.

The ONLY solution I have found is that after doing the first operation, instead of centering X&Y again for the second operation, I leave it where it was and only set my Z height.

This is very frustrating for two reasons. 1, I am never 100% sure that it will actually be on, so I am always having to watch it for the first little bit to make sure. Lots of time wasted. And 2, I have burned through about 3 MDF plates now because every time I want to rerun side b for this product, I need to recut a new section of MDF and start all over again.

To answer some preemptive solutions/questions…

No, I do not move the bed AT ALL in between operation A and B.

Yes, I have made sure to run surfacing passes on my material to ensure that it isn’t the material that maybe is tilted or off somehow.

Yes, I have surfaced the bed of my Nomad to make sure it is square, which it wasn’t when I got it, btw.

Yes, I have made sure that the homing switches are free of obstruction and very clean before attempting.

Yes, I have tried “resetting” the nomad through settings in Motion.

I would love to be able to have dedicated plates for each individual operation to make my workflow smoother. unfortunately, I cant rely on the center of the Nomad staying constant to be able to do that.

How many times did I say ‘operation’? Lol. Felt like a million.

2

You’re re-homing after you got your stock in the pocket?

1 Like
3

I hope I am understanding what you mean… By rehoming do you mean Jogging? Whenever I Jog it wants to measure the tool again and I do that.

4

Or should I be power cycling the entire machine in between operations to “Initialize Machine” again?

5

You’re resetting XY zero? You should just leave that alone.

Above, I was asking if you re-initialized… Sounds like no.

6

You dont need to initalize between sides. The homing is pretty accutate but it can be off by thousands of an inch on initalization.

7

So, my question is then, how am I supposed to create a fixture that is accurate that I can remove and reuse if I can expect the homing to always be off?

Am I asking too much of the machine?

8

Homing isn’t off that much — it should be to somewhere between half the positioning sensitivity of the switches and half a step.

I like to make fixtures which register against a physical aspect of the machine (to place them) and which use a rapid position point as the origin (so that I don’t have to record/enter machine coordinates).

Remember that using the center will double any error — best is to use lower-left corner (first operation), then rotate front–back, and use the same physical corner as upper-left origin (this requires that your stock be adequately square).

9

I don’t know that we are talking about the same process here. From what it sounds like, you are assuming the piece stays in the stock the entire time, which would negate the need for a fixture.

I mill the piece out entirely, then use a fixture to hold the piece for the second operation. Therefore, I rely completely on the bed to know where zero is.

I will try using the lower left corner instead of the center as well to see if that helps keep things more in line.

10

@Wyste Not sure if you saw my reply above. Are you resetting XY zero after the pocket operation, before your start the chamfer op?

11

Hey sorry I missed it! Yes I am. When I dont reset it, everything works fine. However, that seems wrong in my mind. I should be able to always set X&Y and center (will switch to lower left per WillAdams comment) and be back square again if anything were to happen… Like i switch the machine off for the night, or I have an error and pull stop. Or even if I swap the plate. Theoretically I should be able to put that plate back on in the same position and have it be spot on still… Maybe?

12

Anytime you re-initialize, zero is lost. It will be close, sometimes close enough, but likely not exact.

How are you resetting zero at the center?

Then I think your process is good. Don’t reset zero. If you can, leave the machine on overnight.

13

I am using the center preset on the nomad. When I go to set the Z height I click rapid position to the center and zero everything.

I can understand leaving the machine on, but that isn’t a solution I am looking for. And doesn’t seem like a good thing to do long term for the machine.
Also, I want to be able to have a repeatable process between operation 1 and 2 and that would require swapping plates out various times and so I need a constant to come back to that doesn’t change.

I’m going to do some testing tonight to see if I lose zero very badly if I go off the preset lower left corner for zero and then cycle the machine to rehome.

I just need something dependable and I know it’s possible because I have seen so many run production amounts of work off of a machine like this.

14

Doing the pocket to hold the stock is a great way to do it… Just don’t reset zero.

You could also drill a 1/8" hole to use as your zero. Jog until your 1/8" endmill is perfectly centered on the hole and set zero.

15

I have recently worked flipping and lower left works better than center for me, cant explain why it just does. Also I try not to shut machine off or re-home as I have found that the homing switches are not consistent enough for flipping, depending on the project even 100 thou can mess up design. Each time i do write down x and y coordinate just in case and try to ensure homing happens and end results are the same offset .118 for me. Have you thought of using the dowel pin method vs pocketing? May require more workspace tho. You are correct it shouldnt matter but reality is as you are finding out it does. Lastly when I set xy I use my finest tip bit via the manual method. V bits work good to consistently sit on the corner or a 1/16" bit. Just what i am learning on my journey with flipping. Hope it helps.

1 Like
16

I have a couple fixtures that are doweled to the wasteboard, and have zero lines scribed on the base.
Even then, I still check the zero by measuring a feature on the part with a known dimension. And occasionally have to move the zero by a few thousandths.

When I flip a job, I do what Will suggested and use the same “J” corner as the zero for both sides.
so if I Use Left Front Top then flip vertically, the 2nd side uses Upper Left Bottom. If horizontally, 2nd side uses Lower Right Bottom.

4 Likes
17

I use a pin index for this, and have had good success. In the top-side CAD file, place two 5mm holes with say 8mm depth in opposite corners of the stock well away from your wanted cuts and away from any jigging/clamp positions. Bigger dia pins might be better, but 5mm x 12mm is what I have. Drill these holes at any convenient time to your workflow for side 1 - there is some argument saying do it last (if your stock moved at all during side 1 cutting, the holes will still be right, plus the drill/mill is in your collet ready for step 2 below).
In the second side CAD file, keep these two holes in exactly the same position (Vectric has a great facility for doing exactly this - two sided stock features) but flip the CAD to match the direction you will flip the stock. Before you mount/clamp your stock, drill or mill these two 5mm holes into your spoil board or jig board and insert the 5mm pins (I use ground precision steel pins) leaving half sticking proud to accept the stock.
Now you flip your stock (the same way as you planned for in the CAD flip) and it will drop onto the pins exactly in alignment.
The key thing in all of the successful methods described in this thread is that you have to either have exactly symmetrical stock and place your CAD details ‘on symmetry’, or you have to ensure you are always using the same physical place on your stock to reference your zero (say bottom left for side 1, flip so the corner you touched off on is now top left and your CAM reference must be set to that too).
The pin and hole method gives this consistent reference, but the downside is you have to drill holes in your spoil board/jig board and in the corners of your stock on one side. For me this is a price worth paying for not having to worry about errors.
YMMV and your preferred technique too.

4 Likes
18

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