Basic question on mill part setup - part origin

[ctwo]

Rich's comment about engineers really explains the why. Of course if I was creating a drawing, I'd put the origin and dimension from the lower left. I see how that trickles through the process now.

For the sake of discussion, I envision a finished part (a cube) and code supplied to me. The job is to very accurately mill some channels and holes on one (top) side. The problem may present that the outer dimension is much looser, so the lower left corner of the part will never end up in the same spot from part to part. I can see if I rotated the vise and stop 90* CCW, then I'd only have to deal with Z (Now why didn't they put the fixed jaw on the other side?).

How is this usually handled in a production environment, where it seems you'd often have a finished side to work from and a rough cut side? Your work offset would change from part to part if the vise is mounted conventionally.

[Dave_C]

CTWO,

You might be surprised! In a production environment part origins will be set so that each rough block of material is placed in a vise and also against a stop on one side or set in place with some fixture.

Fixturing is quite common and desirable just for the reason you stated about working on a partly finished part.

If each part is machined from the same setup, the part zeros should still be what they were when the part was started.

But how precise are we talking about? If there has to be an exact match to a finished surface then either a fixture that holds from a finished surface on the part or plan on probing a lot.

If you can duplicate the original setup, you can finish the part.

At least that is how my poor brain works.

Dave C.

[ctwo]

It was just a rhetorical part. I think I will ditch the conventional vise orientation on the CNC and rotate it. This will allow me to reference the origin and machine in quadrant 1, the way everyone is making their drawings and code.

[GlennW]

ctwo,

Stan Dornfeld was a member here and used to manufacture these vises.

http://sandiegocnc.com/Quad-I,+Dornfeld ... orkholding

This may clarify what you are referring to.

I don't have one nor have I ever seen one, but I recall conversation about it.

Stan retired a few years ago and I don't know if anyone took over manufacturing them or not.

[Harold_V]

Harold, I don't understand the comment about the axis's being switched ?
It has nothing to do with axis revisions, but with origin location .

What I'm talking about is the way drawings are presented to the machinist. It is commonly accepted that a part is looked upon as north (up) as being the Y axis. If one rotates the part, it then becomes the X axis. While that is something I've had to deal with countless times, I do so by re-dimensioning the part, switching datum points. By holding dimensions instead of abusing tolerance, that works perfectly well.

My point is that when you introduce ANYTHING that may offer the risk of confusion, it's not a good idea. Machining a part by rotating offers that very thing---the opportunity for error. Mind you, I'm not suggesting that it doesn't work. It does. I'm also not suggesting that working with all positive numbers doesn't work---it does, too, but for a guy who has spent more than 50 years using the top left portion of a part as a datum point, switching offers risk of making errors (don't lose sight of the fact that I was a manual machinist, not a CNC machinist). I work as I do and do so with virtually no errors (or at least I used to). I'd not enjoy trying to re-learn everything because I chose to rotate a vise.

There's one really good reason to use the top left corner as a datum point. That's where the fixed jaw is located. The fixed jaw is a constant, while the moveable jaw is not. If one does second operation work, using the lower left hand corner can introduce error due to stock (or parts) not being consistent. That's a good case for turning the vise and setting a stop on the near side, which would be less than a good idea for a manual operation.

By machining as I was trained, I can always put a part back in the machine and know that I am properly oriented. I'm not willing to give that up.

The transition to CNC has resulted in some changes in the way things are made. It has also resulted in changes in the types of tools used. For example, I spent 26 years of my life in the commercial shop and never once saw, let alone used, a spotting drill. Center drills were the accepted cutting tool for spotting holes. They work perfectly well for that purpose. Note that I'm not arguing against spotting drills---just defending a practice that was universally accepted long before spotting drills were introduced to the shop.

Harold

[Lew Hartswick]

From a manual control viewpoint; I hardly ever look at the sign on the readout on the Bridgeport. I just KNOW which direction I'm going to move and do so.
...lew...

[ctwo]

I'd not enjoy trying to re-learn everything because I chose to rotate a vise.

There's one really good reason to use the top left corner as a datum point. That's where the fixed jaw is located. The fixed jaw is a constant, while the moveable jaw is not.

Harold

Harold, I think rotating the vise means just the vise. The work orientation would remain.

Take letter engraving. All dims start at the lower left so the engraving is all pos XY on the drawing. Now the engravings go onto stock that is 1/2", 1/4" 3/4", or other random widths for the letter heights. Every time you change letter size or your stock size, you have to relocate the origin to run the code.

[Harold_V]

Harold, I think rotating the vise means just the vise. The work orientation would remain.

Thanks. I wasn't seeing it from that perspective, and for CNC, that makes sense, although when I engraved the faceplates for my lighting system, I still used the upper left hand corner. Old habits die hard with me.

Harold

[Tom - AMS]

I own two CNC production machine shops. We do a lot of 3, 4 & 5 axis milling. Where the part origin(s) is/are doesn't make us any difference, because normally the raw stock is extra big with plenty room for the finished part. In our world, a little extra mat'l is cheaper than set up time and with CNC, buszzing off an extra 0.100" is as quick as blinking an eye. We just look at the drawing, and set X-Y-Z-A-B =0 with a digital probe to where ever the CAD/CAM guy selects, or if we're programming at the machine, we pick the origin for whereeve makes the most sence for the entire machining / work holding strategy. In most cases it is the upper top left, if its vise work. Working with both positive x and negative y values (and /or even negative x) is "normal", and no big deal, even for an old guy like me with 50+ yrs of manual machining Usually we use negative Z values, setting Z =0 on top. In some cases, we'll set Z off the bottom. For example if the first two ops are to face a part 0.010" and cut an o-ring groove, say 0.070" deep from that face, in 1/2" thick rough stock, we'll set Z at -0.500 off the bottom. The 1/2" raw stock typically varies from -0 to +0.015. this way it doesn't matter how thick our original set up piece was, we'll always have our faces surface at Z -.010, and the o-ring groove will always be, incrementally, 0.070" deep.
Alternatively, if we already have a finished bottom, we often use it as Z=0 and work with positive z values. Like instinctively knowing which way to crank the handles on a manual mill, its not a big deal working with +/- values - as long as you stay consistent for that parts run
As mentioned in a previous post, on some complex jobs we may have more than one Work Co-ordinate System ( G54, G55, etc up to as many as 200 WCS). Or its common to have 3 or 4 vises on the table, each with its own WCS running the same part, or doing a 2nd, 3rd, 4th operation. we load & unload vises ( or pallets) on the fly.
With all work holding, we initially probe the vise jaw or other reference surface on a fixture or part work piece to establish Co-ordinate System Rotation angle. (CSR = automatic tramming to the X or Y axis). Additionally, we can use G68 / G69 to do dynamic CSR withing a program. If, for example, the first op req'd clamping the stock in the vise in a traditional manner ( jaws parallel with X) and then for some stupid reason the CAM guy has the part held 90° to that for the next op, without any other reason to re-clamp the work, we simply add a G68 or 69 to rotate the WCS 90° for that operating, and avoid having to remove and reclamp the part. Our mills also have Z-axis CSR, where we can plop an odd lump of metal in a vise, with say a top surface at a rough 15° angle to XY plane, probe each end, and set the Z axis to follow it at whatever CSR angle we wish ( level or 0°, or a true 15° or any other angle less than 90°. This works best with ball nose end mills, but with careful programming can also be used with sq end miles and produce a nice flat surface.
Often with rough stock, the origin is in the center of the work piece. In most cases there's never a reason to remove it until several finished sides are machined. Typically we just use stop(s) set to locate each piece. In some cases where the rough stock has very little margin for cleaning up at net shape/size, we'll piggy-back a simple probing cycle on the parts G-code to find the center of the stock. This is only done when the raw stock has very little margin for net shape. For example if we have a raw 2.010 L x 2.006 W x 2.020 H "cube and we need a 2 x 2 x 2 cube out of it, well probe the center in X & Y, and set is at X = 1.005 Y = -1.003, then probe Z mid point and set it at Z -1.010. In practice, we usually don't have to center in Z. Most raw stock is thick enough; probing for Z center is usually only needed when some jack-wagon saw cuts the raw stock too close to net size.
Also, unlike manual milling's vise work, most of our CNC vise work uses what is called carrier (or flip & face) work holding. We grip only about 1/16" high off the bottom of the stock, so we can zoom around all 3 sides, often using a larger piece of raw stock for multiple parts. Then we have soft jaws machined to accurately locate and hold the part(s) when flipped over. We either face of the 1/16" thick "carrier" material, or we machine features into the bottom of the part as needed. Like soft jaws for lathe work, soft jaws for CNC milling make things easy and accurate. We also us a lot of pallets with dowel pin locators, or the part is DFM with dowel or other locating features. Unlike many manual milling jobs, we typically don't have to worry about always using the fixed vise jaw to achieve most accurate results. In the rare case we do, we just go ahead and include a 10 to 15 sec probing cycle, reset the origin as need and will be dead-on target.
Homing switch functions varies from machine to machine - but for most modern machine like ours, their big advantage is they let us shut down in the middle of a job, say at the end of the day, and then crank up the next day, home and pick up where we left off in the middle of the job. Or we can use several WSC ( G54, G55, etc) and do a quick one off job, in the middle of another batch, without having to reset that batch's origin. They let the machine remember exactly where the last x-y-z-A-b =0 was set for each WCS in relation to the Machine Co-ordinate System. On all our mills the Home position is max positive values for all axis, minus a few dozen reverse ball screw encoder counts. They move 'til they hit a limit swithc then back up a pre-set number of encoder counts, and then compare that position to a previously stored position - if they do not match, it alarms an error message. The cure is often just wiping a chip off the limit switch an re-home that particular axis.
regards,
Tom -AMS

[Big Rack]

What little I know about CNC milling tells me it's all at the preference of the programmer who often is not the guy at the machine. In my opinion the programmer must include a accurate and complete set up sheet. makes it much easier if you have more than one guy running the job.
If it were me I'd use the same place always, and I would use it for x,y, and z. If a vise, the the fixed jaw of a vise. More likely I would use a tooling plate instead of T slots to mount everything with a precise point always in the same place to set zero from. This way the origin is always the same for every job. While I used to program my lathes we used to have our mills programmed by an engineer. Always seemed to me they made it a lot harder than what it had to be.

[ctwo]

I have so much to learn about the basic CNC workflow and that is a big part of the question. Most often, I will likely be the stupid cam guy, but I will come to an accord with that. For now, I am often working with downloaded gcode programs or other posts from free SW, and functionality (and knowledge) is limited. Now that I know that there may be a CSR function, I can explore that. I also need to figure out how to set up WCS or work offset systems. I have been playing with Mach3 so info on this will be abundant. As a hobby, time is limited so I tend to have to relearn a few lessons each time I get into it.

Thanks for all the info.

Edit, ah now I think I can use the upper right jaw for a reference and use G68 R180... Have to test it out.