[SCzEngrgGroup]

I've always used what I suspect is the most common convention for picking my fixture coordinate origins:

• For parts in a vise, I generally zero X/Y to the left front corner of the fixed vise jaw
• For parts in a fixture, I generally zero X/Y to the left front corner of the fixture
• For Z, I've always set the Z fixture zero to either the top of the stock, or sometimes to the top of the finished part

Recently, I've been setting the Z fixture zero differently - I'm finding it actually more convenient to set the Z fixture zero to the BOTTOM of the part. This has several advantages:

• It no longer matters if the stock is slightly thicker, or thinner, than expected. Setting the fixture zero to the top of the stock, unless it has been "prepared" to the exactly correct thickness, will not necessarily give the correct final thickness for the part. The first operation on each side is always to face-mill it to the expected thickness, as measured from the bottom of the part, so the parts always come out exactly the right thickness.
• Previously, if I machined the top and bottom of a part, I would have to zero G54 for the top of the stock or part, for machining the first side. I'd then have to use G55, with a different Z offset, for machining the second side, since the part thickness is generally changed by the operations on the first side. With the new approach, both top and bottom machining operations can use the same Z offset, since the bottom of the part is always in the same place, be it on a fixture, or in a vise. This is true even if the second-side operations don't clamp to the original bottom of the part, which is often the case for me. I can now perform most jobs with only a single fixture setup (G54), where I sometimes needed as many as four before.
• I often end up doing the second-side machining with a very small portion of the part held in a vise or fixture, with the tool getting very close to the vise jaw or fixture (sometimes only a few thou clearance). Making sure there truly was clearance meant knowing exactly how thick the part really is, how much is below the vise jaw or fixture, and how deep the cut was, then doing some math. But, with the new approach, I simply need to look at the depth of the cut, which directly gives the height of the tool tip above the reference surface (parallel, fixture, etc.). If I know there is 0.125" clamped in the vise, any cut that goes below +0.125" will hit the vise. Much simpler, and no math required!

Regards,
Ray L.

[kvom]

For 1-off parts lately I've been drawing them centered on 0,0 and then zeroing to the center of the stock.

[LeeWay]

I only have one production part that is machined on more than one side. I do set my zero's much the same way you used to, Ray.
I have done parts like Kvom as well. One off's especially if I will machine the back side off. Then you get a perfect profile.

You loose the Z position when you do 3D parts by zeroing to the top, but if all tools are in the tool table, then everything SHOULD work out fine. Assuming all goes well. If the top is gone though, you may be in trouble if you break a tool.

I set my tools off the mill with a digital height gauge, so not too big of a deal for me. Those that use a probe might need to consider doing what you are doing now, Ray.

[AUSTINMACHINING]

Like they say,, "many ways to skin a cat"

I have yet to bolt anything to the table other than a lathe chuck holding a drill bit. All my fixtures are small enough to fit in the vise (so far). Seems like all my parts have to be rotated 4-5 times. Here's the strategy I use in Solidworks.
I have a template file that already has 6 "display states" The display state control what is visible on the screen, parts,vises coordinate systems etc. The template file has 6 vises with 6 coordinate systems all located on the left front edge of the fixed jaw. For operation 1, display state 1 is active showing the part and vise #1 only. The part is mated to the vise as needed with parallels etc. Once the simulation is complete (no collisions etc), I activate display state 2. Now, only the part and vise #2 and coordinate system 2 are visible. I mate the part to vise #2 to machine the next set of features as needed and simulate. I repeat the process using the various display states as needed.

Remembering that all the coordinate systems are referenced to the same location on the vise, I post process all the "jobs". When it comes time to machine, I touch off the front left edge of the vise (G54) one time.
I can now flip the part around in the vise multiple times as needed until the part is complete. No need to indicate location more than once.

Hope this helps/makes sense.

Matt

[mklotz70]

Ray....just to be clear.....is the middle line correct?


For parts in a vise, I generally zero X/Y to the left front corner of the fixed vise jaw
For parts in a fixture, I generally zero X/Y to the left front corner of the fixture
For Z, I've always set the Z fixture zero to either the top of the stock, or sometimes to the top of the finished part

I understand the left front(being the clamping surface) corner for the fixed jaw, but I would have thought that with a fixture, it would be the left REAR corner. If it's a typo, cool.......if not, can you explain why you use the front(being the side that contacts the movable jaw) corner for a fixture. I'm still a noob learning this stuff, so this is certainly more of a question than a correction!!

Your change in how you set Z makes a lot of sense. I've seen a lot of stuff reference the top of the part and it just didn't seem the best or easiest way to do it. I figured it would be come clear when I started setting up parts, so I haven't questioned it yet. Thanks for the information and explanation! I'm going to be needing this soon.

[SCzEngrgGroup]

Mike,

Fixtures, in general, are not held in a vise at all - they're bolted directly to the table.

Regards,
Ray L.

[mklotz70]

Ah....thanks!

So do you use the front left corner because it's easier to get to?

If the fixture was being held in a vise, would you still use the front corner? I would think that if the fixture accurately registered to the fixed jaw, you could keep using those X/Y positions and just change the Z.

[LeeWay]

I will have to redo most of my machined parts in F360 to take advantage of adaptive clearing. For some reason, many of my part zero's in the vise is either front left or right. Probably a legacy thing from my old mill. It has the stepper motor out front, so makes it farther away to zero to the fixed jaw. I will get everything on the same page now and zero everything to the same side of the fixed jaw. Then all parts we machine that day will have the same X and Y zero point. Only the Z would change.
I do have two parts that are mates and are 5" long finished and both ends get machined. Those parts hang off both sides of the vise.
They both still have the same starting points though.
I need to set the final position before rewind to zero X and Y and .1 on Z. That way I know exactly where to clamp the next part.
I considered using a vise stop instead and actually built one, but since both ends get machined, it wasn't designed to easily get out of the way while maintaining position.
So, while there are certainly valid reason for some type of logic behind setups, different parts may have different requirements, so not everything fits in the same box.

[mklotz70]

Since your vise stop would have to be out of the way, could you use a 1" reference, like the one that comes with micrometers? You could use that to set the part exactly 1" from the vise stop....you'd have room to mill the end and your endmill would be up and out of the way. Is that a practice that's just not accurate enough. I understand stopping your cutter and using it to reference the next part.....I do that on the lathe.

[LeeWay]

All it has to get is close. We cut the blanks about 1/8" longer than needed. It's not even critical that the back or left side on each gets faced off. The front part or right end has a radius profile, so it is the important end to get lined up right.
These are the parts that we make the most of. They have the most holes and tapped holes. It is easy enough to just add that Gcode at the end of those programs and eyeball it, than it is to setup the stop thing.

There is a way to make the stop swivel out of the way if the end accuracy is critical. Have the stop swivel between two nuts. Then have the adjustment on the threaded rod that the stop is on. Bolt that in a fixture at the back of the vise. Then you have it. Lift the stop, place the part and clamp down. Then drop the stop. I have given it some thought and I think that is one of the points in Ray's thread here. It might make things a little easier on us if we give some thought and apply some logic to our setups for various parts.

[mklotz70]

Nice....I like what you described for the stop. Thanks!

[rowbare]

Setting Z = 0 to the bottom of the part is especially good if you are hand coding. You know that you should never see Z < 0 anywhere except for maybe drill tip clearance and some final profiling ops.

If you have room on your fixture stock and you have a probe, it is useful to pocket a circular hole and define its center as 0,0 and then go on to mill the rest of your features in relation to that. It makes it really easy to zero your fixture. Clamp it down, run a centre circle probe routine, zero your x,y axes. If your your pocket is the same as your fixture, you can probe your Z too.

bob

[amish_rabbi]

is there any reason to not use the following strategies?


•For parts in a vise, I generally zero X/Y to the left front corner of the fixed vise jaw--z on top of vise jaw
•For parts in a fixture, I generally zero X/Y to the left front corner of the fixture--z on top of fixture plate

[tmarks11]

is there any reason to not use the following strategies?

I usually do exactly as you have said.... but...

If I have a double sided part, and am not using a fixture plate, I keep the X,Y coordinates at the same location on the part.

IE, origin starts at left back corner of part (which coincidently is usually left front corner of fixed jaw). (z axis on surface of part)

When I flip it (long end for long end), the X,Y coordinate is now right back corner of part (z axis on new surface of part).

This elements any possibility of the stock being a different length than what I modeled as my stock in HSMWorks from causing the second side cut from not lining up with the first side.

It is embarrassing when you modeled at 6" long chunk of stock IN CAM when you generated g-code, but you were lazy and used a 6.3" piece of stock without cutting it to size. If I kept the coordinate at the left front corner of the fixed jaw of the vise, the second cut would be misaligned by 0.3".

Clear as mud?

If I have a fixture plate that lines the part up on both sides, than I x,y,z off the fixture plate back left corner as previously discussed.

[SCzEngrgGroup]

When I flip it (long end for long end), the X,Y coordinate is now right back corner of part (z axis on new surface of part).

Or, when you flip it, keep the origin on the left end of the vise jaw, but line it up to a machined feature on the part. This is how I almost always do it.

Regards,
Ray L.