Part location

[Brian Orlando]

I've been reading a lot and watching tutorials but I never see anybody mention how and where the locate the part on the cnc table. After you create a file and tool path how do you determine where you locate the work piece? Do you put it in a corner or the center? Am I being anal her or what?

[Jerome Stanek]

It depends on how you have your table set up. Most use a corner mine is set to use the lower left corner while standing in front of the x axis the long axis.just as you see it when you do your drawing. Some times I cut preprinted stuff and have to use the opposite corner and the Y is backward. At where I work that machine uses the upper left corner

[Bob Savage]

Unless I'm misunderstanding the question, assuming the part is smaller than the table (i.e. not the same size) you can locate it anywhere you like. From there you set your XY0 coordinate so that your machine knows where the part is on the table. The XY0 coordinate will depend on how you set the job up in your design software. I generally use the bottom right corner of the material or the center, depending on what I'm cutting.

[Brian Orlando]

What I'm thinking about is taking a pre cut to size cabinet side and only machining the dados, shelf pin hole and hinge holes. Right now I'm cutting parts on vertical panel saw, Line drilling on dedicated machine and running dados on the table saw. I'm thinking about getting a 4x8 cnc with atc or x3 if funds and lagistic's allow, where I could cut and machine the parts . I also want to be prepared to deal with a smaller machine where I have to do parts one at a time and having to do multiple manual bit changes. I might be over thinking this. The majority of my work is cabinets. How are you guys handling this? I might have to pony up a lot more money for the larger machine if it's to time consuming to do it one part at a time. Thanks for your input here guys.

[Jim Underwood]

All CNC machines have a x zero, y zero point for where programs originate. If you have a controller for your x, y, and z axis, you may even have a field in the software for setting it's location. Also many machines with vacuum hold down have location pins that pop up when the bed or gantry reach the x0, y0 point. This is so you can locate a part for operations to be placed on it, or so that you can place a new 4x8 sheet for a nested set of parts to be machined and cut out.

And no, you're not being anal. That's a very good question that absolutely needed an answer.

[Gerry Grzadzinski]

What I'm thinking about is taking a pre cut to size cabinet side and only machining the dados, shelf pin hole and hinge holes.

In high production shops, CNC's are usually used two ways.

1) Nested manufacturing, where the CNC does all the work in one operation. Parts are nested in full sheets of material, and come off the machine ready for edgebanding or assembly.

2) Parts are cut on a saw, and the CNC is used for all other operations. On industrial machines, pop up pneumatic locating pins are used to position your parts at X0 Y0.
Since I've used this method for many years in my day job, I set up my home machine similarly. Rather than pop up pins, I've mounted fences along X0 and Y0, to accurately locate my parts. After homing the machine to the home switches, I trimmed the fences exactly to the zero positions, so I have a very repeatable zero position. I usually hold my parts against the fences with cam clamps.

I almost never change the zero position on my machine. I have my machine table drawn in my CAD program, so if I want to cut a part away from the table, I just draw it in my CAD program exactly where I want to cut it. So I turn it on, home it, and it's ready to go, with X0 Y0 in the same spot, every time. This is how it's typically done on the big industrial machines, where time is money. When you have hundreds of parts to machine, you can't waste time setting the zero position with every part.

[Neal Schlee]

I have a couple of Multicam's, they allow for up to 5-soft homes to be set. This allows for running the same or a different file in various locations on the table. For instance, if you have a 4x8 sheet of ply and need to cut multiples of the same part, you can set the soft homes to utilize the whole sheet without having to create a new file. Also, if you have a multi-zoned vacuum table you can use this feature to run parts continously, while one home is cutting in one vac zone you can be changing the part at a completed vac zone while the machine is cutting, this minimizes machine down time. Our MC's both have dual Z's and when production cutting parts with the multi-zone technique it keeps the operator hoppin' and really pumps out the parts.

Neal

[james mcgrew]

wincnc on the CAMasters have 10 to 20 saveable home positions, you can set one for doing cabinet sides and another for a repeatable 3d,

i have been down this same road and went small machine, within six weeks i realized the mistake i made and bought a 4x8, 4 months later an X3 which is still my primary machine, feel free to call and i will show it to you, as a cabinetmaker find some way to get a tool changer of some kind,,,, a single head machine is not impossible but it is one i wish i had avoided.

[Bob Savage]

I almost never change the zero position on my machine. I have my machine table drawn in my CAD program, so if I want to cut a part away from the table, I just draw it in my CAD program exactly where I want to cut it. So I turn it on, home it, and it's ready to go, with X0 Y0 in the same spot, every time. This is how it's typically done on the big industrial machines, where time is money. When you have hundreds of parts to machine, you can't waste time setting the zero position with every part.

This is an interesting concept. How are you measuring at the table to locate your part in the cases where you're cutting a smaller piece in the center of the table? Also, how would you measure for indexing something where you're flipping a smaller part that's somewhere other than your XY0 location for two sided machining?

I'd love to save time by not having to set XY every time I cut something new.

[Jim Underwood]

For reverse operations, in your situation, I'd cut an "L" shaped piece to exact dimensions. The inside corner will have a small hole centered on that intersection, so that the radius will not interfere with the corner of your part. Then you output your reverse part at the exact location of that inside corner. This does two things, one, it helps keep the part from moving, and two, it locates that part exactly.

The way I do it is to locate the part in the correct orientation, and place it against our locator pins. Then when you hit the vacuum switch, the pins drop out of the way, the vacuum holds the part down (hopefully) and then I run the reverse operations program.

Every program you draw will have a x zero, y zero origin point which should correspond to your bed. I'd just draw the part about 1/8" from that corner both directions so you have a nice trim amount.

[Jerome Stanek]

I always use the same corner to locate my parts. If I want to cut a part in the center of my table I just move the z to where I need it. and that becomes the x0 y0

[Mike Heidrick]

I have spots on my table that are set to fixturing spots (G54-G59) in Mach. Most of the time I use those. I always home first thing when I start the machine. The fixture spots are always exactly in the same spot.

I use two touch plates and the Mach Blue Big Tex screen. I initial tool zero with the first bit and it touches off on the plate I place on top of my work and then it touches off on a fixed bed plate on the table away from my usual cutting area. I cut the first tool's path, it finishes and comes to home, then I change the bit and hit tool change and the bit moves and touches off on only the second fixed plate and then comes back to home, load the new path and hit cycle start. I was using a quick bit changer on the router and I could swap tools and be cutting the second path in under 30 seconds. With the spindle it is about 45 seconds. At that speed its hard to justify ATC for my shop.

The cost - $.50 of copper clad plastic, $3 in wire, and one input, and a free mach screen and 3 mins of script editing. A Chinese ATC spindle is over $2K new and a HSD or Columbo ATC setup is big money.

[Gerry Grzadzinski]

This is an interesting concept. How are you measuring at the table to locate your part in the cases where you're cutting a smaller piece in the center of the table?

My table also has a grid of about 120 T nuts in it, which are also shown in my cad template. I locate the part where I want it in AutoCAD, and drill 1/4" holes where the T nuts are, and bolt it into place with 1/4-20 bolts. I place it against the fence to drill the holes.

Also, how would you measure for indexing something where you're flipping a smaller part that's somewhere other than your XY0 location for two sided machining?

I'd probably bolt down some scrap MDF and drill some holes in it for locating pins.

[Bob Savage]

My table also has a grid of about 120 T nuts in it, which are also shown in my cad template. I locate the part where I want it in AutoCAD, and drill 1/4" holes where the T nuts are, and bolt it into place with 1/4-20 bolts. I place it against the fence to drill the holes.



I'd probably bolt down some scrap MDF and drill some holes in it for locating pins.

I like it... thanks for the tips.