Model too long for my CNC bed

[paul.hermans]

Hi everyone, 

I am new to Fusion 360 so I may be approaching this all wrong and am hoping someone can point me in the right direction.

I have a design I need to mill into a long board. The stock is 9.25" by 48" but my CNC is a shopbot desktop which can only have 24"x18" useable area.  The pattern is a flower, and the stem is roughly 26" long.  Of course it needs to be in the middle of the stock.  

My plan was to mill it in two steps, while moving the stock in between.  This worked ok, but the alignment was slightly off after I moved the stock so I am wondering if there is a better way.  I used the CNC to drill a few alignment holes, but it was till off by about 1/16" (visible in the stem).  Is there a good way to setup for a material move, or should I break my solid body into 2 pieces etc?

Not sure how to explain it I have attached the file in case someone want to take a look.

Thanks for any advice you can give.

Paul

[RandyKopf]

@paul.hermans

There is likely more than one way to deal with this. But here is one attempt. 

This is a very common problem that anyone who's been in a shop has encountered.

The concept you applied in Fusion is solid.

It's the execution on the machine that is giving you problems.

can you measure the mismatch with a precise tool like a caliper?

-

I recommend a calibration cut.

1) Cut the bottom segment as you did.

2) Try moving the part as accurately as possible.

3) Change the Stock to Leave on Flower Top to little more than the mismatch you've seen.

4) Cut the Top. (Because of tool size and stem width I could only leave about 0.045")

5) After rough cut measure the mismatch.

6) Create a new SETUP and shift the origin by that amount you are off. 

I did this in the attached model to show how to do it. And I added verbiage to explain it.

7) Cut the FLOWER TOP to finish size.

8) Use fine sandpaper. If you did it right that is all you need haha 

Let me know if you need any clarification.

[LibertyMachine]

When you drilled your first set of alignment holes, how did you go about locating off if them in the second setup?

How are they off, laterally?

Do you have your stock riding against a rail so you now it's running true to the X axis (or Y, depending on the setup of the machine)

The way you have it setup is correct. I'm looking more at the mechanics and machine side solutions

[paul.hermans]

Randy,

Thanks for the detailed instructions.....one question that I have struggled with related to this idea is how to move the origin precisely when in the CAM setup?  I can pick points etc, but there doesn't appear to be a way to simply move it without first going back to my MODEL space and adding some sketch element. Is that accurate?  I think I will try what you suggested on some scrap to make sure it works.

Thanks for the suggestions.

[LibertyMachine]

That is the only way to nudge over a work offset. 

[paul.hermans]

Good question.

When I first mounted the stock on the table it had no holes in it whatsoever. I made all the holes in the model. Once i had zeroed everything, my first operation was to drill the four lower holes through the stock and into the scrap table so I cut put an alignment pin in the holes when I moved them.

I then ran the lower section of the flower....my parameters were a little off and it took a while but it worked well.

Then I moved the stock by putting 2 alignment pins in the first two holes (1 left and 1 right side).  I then placed the stock on those pins by aligning the 2nd holes......then I drilled the third set of holes and moved the stock again.  

Then I ran the stem of the flower and found it was off about 1/16 or so. This surprised me since the CNC had drilled all my alignment holes in the correct places.

Then I ran the rest of the top half of the flower.....all worked well except the left/right alignment was slightly off.

As I write this I am wondering if it would work better if I did the following:

1) Mount a new scrap table top with no holes etc in it.

2) Have the CNC square the table etc.

3) Mount the stock as close to square with the table by lining up the long edge.

4) Have CNC drill holes along the left edge that go all the way through the stock and 0.3 into the scrap table. These are guaranteed to line up as they were made with a single operation. I would make them at these locations:

     (0.5, 1)

     (0.5, 9)

     (0.5, 17)

7) Leaving the stock in place, have CNC mill the bottom half of the flower.

8) Dismount the stock. Move it down 8" so that the hole that was originally at (0.5, 9) is now at (0.5,1) and the hole originally at (0.5, 17) is now at (0.5, 9)

9) Drill a new hole through the stock at (0.5,17) but don't go into the scrap table.....theoretically this hole should line up with the one previously drilled in the same location.

10) Dismount the stock, move it down another 8" so that the hole originally at (0.5,17) is now at (0.5, 1) and the newest hole is at (0.5, 8).  

In theory this should keep the stock perfectly (or very nearly perfectly) aligned but shifted by 16"

I should mention that the stock is just poplar wood so easy to sand the surface a little if needed.

11) Mill the top half of the flower stem, but only .002 deep to see how it aligned with the previous piece.  If it is good, mill it again full depth. If not, then I have to adjust the origin somehow.. I can think of two ways.

1) As suggested in another comment, go back to CAM and move the origin....this is a pain because it is hard to precisely move the origin in Fusion 360.

2) Move the CNC back to 0,0 and manually move it slightly left/right, forward/backward to adjust for the mis alignment. Then make this new position = 0,0

Either way, rerun the flower stem at a depth of 0.004 or something small.....see if It lines up better now. If so, mill full depth, if not so it again.

Do you see a problem with this process or a better way to do it?

Thanks

Paul

[RandyKopf]

@paul.hermans

CALIBRATION CUT ADJUSTING A COORDINATE SYSTEM

To shift a coordinate using a sketch is a viable method. It seems like a mental hang up for you that it's not achievable from CAM directly.

Well I do this at the company I work with as standard practice with Mastercam. Why? We make fixtures that are made up of many parts. They are assembled and have a stack up of error. We inspect the fixtures using the origin that will be used to trim the part on our 5 Axis CNC router. And we measure to key features like Datum's that the part is held against. We then strip the error out of the model. And our preferred method is to use a 3D Sketch for XYZ Shifts. And establish a corrected origin. We have a rabbit trail to show exactly  what direction we moved. And the values correlate with our inspection report.

YOUR NEW PLAN 

So I read that plan and it seems to make sense. It makes you think something you had previously used was assumed square and was not.

AN ALTERNATE METHOD I USE AS STANDARD PRACTICE.

Many times when reorienting a part we make sure

1) Make a cut made on the outside of the stock.

2) We also put in a location hole in proximity to the zone we would continue the cut. (This case put it near the stem joint or in the uncut stem.

3) We move the part

4) We indicate that cut edge.

5) We indicate the hole and use it as our origin for this next process.

6) This way your not moving an origin in CAM. but using one that was established by prior CAM and later setup.

[daniel_lyall]

just grabbing a feature that already exists, will only be out if it is in the wrong places to start with. iT is a good way to do it if you lose power or your origin you just reset your origin to a feature and indicate to it.

A hole is a good feature to use as it gives you a X and Y position, a sketch is just as good

[paul.hermans]

Hi Randy,

I can do make the adjustment to the origin in the sketch, but I am confused as to why this happened in the first place.

In theory, the method I used should have kept it aligned correctly but it didn't and I don't understand why not. 

I don't get to use the CNC every day as I am a teacher and have other classes to deal with, but I will try your method and let you know how it worked out.

Thanks again for all the advice.

Paul