Floating edge

Anybody ever confirm this theory or is it just bs? I have one operator on my Makino a51's that complains about floating edge. We are running common fixtures and AFAIC if the saw cut, and extrusion size is good the concept of a floating edge is irrelevant. I was always taught the 3-2-1 rule for workholding, so I've always perceived that as bulletproof.

please explain floating edge theory. I googled it and got nothing.

Yep, I figured that was the case. The floating edge is measuring off a non machine datum, but if the model reflects a nominal part, and the blanks themselves are nominal it sounds like an excuse to run bad parts. Essentially if my datum is the bottom left of a rectangle and the dimensions are called out from the top right of it the top right is a floating edge. Does that make sense?

Plouch16 said:

Yep, I figured that was the case. The floating edge is measuring off a non machine datum, but if the model reflects a nominal part, and the blanks themselves are nominal it sounds like an excuse to run bad parts. Essentially if my datum is the bottom left of a rectangle and the dimensions are called out from the top right of it the top right is a floating edge. Does that make sense?

Click to expand...

It makes sense, but your Operator is probably right, especially if you're machining extrusions. That is terrible practice.

I'm not sure what the 3-2-1 rule is either...

My personal philosophy - setup the part - including fixturing locations, and work offsets - as the part is drawn. If the dimensions are drawn from one edge, then that edge needs to be qualified, it needs to be fixtured from that edge, and then the work offsets need to be set at that edge as well. That constrains all dimensions to the known location, physical location of the part.

It sounds like you're doing the exact opposite. Ever heard of the "stacking of tolerance" theory?

Jashley73 said:

I'm not sure what the 3-2-1 rule is either...

My personal philosophy - setup the part - including fixturing locations, and work offsets - as the part is drawn. If the dimensions are drawn from one edge, then that edge needs to be qualified, it needs to be fixtured from that edge, and then the work offsets need to be set at that edge as well. That constrains all dimensions to the known location, physical location of the part.
It sounds like you're doing the exact opposite. Ever heard of the "stacking of tolerance" theory?

Click to expand...

3-2-1 just refers to 3 planes of restriction for workholding. Some of the parts cannot be fixtured on those edges due to the common fixturing. These parts have been this way for a decade so it is usually easier for me to move a hole .01 than have QC redraw every single part. As far as stacking of tolerances I thought that mostly only applies to assemblies?

litlerob1 said:

It makes sense, but your Operator is probably right, especially if you're machining extrusions. That is terrible practice.

Click to expand...

Unfortunately the extrusion and saw cut tolerances are +/- .015-.020. So you can see how that variance poses a problem.

Hi All:
Sure, you can make the claim that all needs to be referenced from the drawing datum but that implies that the drawing datum was intelligently chosen in the first place, and also that it is a reasonable datum to fixture from.
Sadly I have seen and you all have surely seen too, some spectacularly idiotic datum choices in our careers.
So a universal rule like this, to my mind is a poor rule to follow slavishly.

In that regard GD&T helps a bit because it forces the engineer to consider his datums less arbitrarily, but even with GD&T rules to follow I still see a lot of pretty strange stuff and if the rule of inspecting in relation to the order of the primary, secondary and tertiary datums is followed you'd have to do some pretty weird fixturing to get your part up on the CMM.

So perhaps the OP can be forgiven if the fixturing he's chosen follows a sensible manufacturing plan as opposed to a totally loopy scheme the engineer didn't properly consider when the part was dimensioned.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

Thanks for the understanding. I'm coming from optic mold making to electrical connectors on 100 something different pallets, so I have inherited quite a bit.

For building fixtures you account for 6 degrees of freedom, those being motion in all three planes and also rotation about all three axis’s. Makes my head hurt…

Never heard the floating thing either, but if it means you leave room for oversize stock in your fixture I guess that’s obvious???

Good luck,
Matt

I have never heard of floating edge or 3-2-1 either. How many sides of saw cut are you using as locating edges?

We've all located parts on one surface and machined features that were dimensioned from a different one. I do extrusions that are defined centerline symmetrical and I locate them from one edge. Obviously a change in material size is going to have an effect.

If the variability of the material exceeds the positional tolerance of the features to be machined, you have to grade the blanks by size and shift the work zeros accordingly. Or fixture it in a way that the variability is not a factor.

I think dimensioning off a “floating edge” is fine as long as that surface is qualified during machining...just like you would in a VMC - If Z0. is the top of a saw-cut part you would “qualify” it by face milling to Z0. after ensuring the part is ALWAYS saw cut to at least .001 talker than the finished length.

A great primer on fixturing:

Locating & Clamping Principles | Carr Lane

guest said:

We've all located parts on one surface and machined features that were dimensioned from a different one.

Click to expand...

Plus we've probably all run into parts where the drawing switches datums depending on the view, or better yet when features are dimensioned from different datums in the same view.

Plouch16 said:

Anybody ever confirm this theory or is it just bs? I have one operator on my Makino a51's that complains about floating edge. We are running common fixtures and AFAIC if the saw cut, and extrusion size is good the concept of a floating edge is irrelevant. I was always taught the 3-2-1 rule for workholding, so I've always perceived that as bulletproof.

Click to expand...

I think you need to clarify the question, because I'm too stupid to understand.

What "theory" are you trying to "confirm"?

321 being 3 Axes, then yes I agree with that.

If you need to stop off a plane that is not a Datum, then that Datum still needs to be established/machined/qualified somehow, like the Nerd said. If you are running one of a thing, using a theoretical is okay, but if you are running a Million things (Extrusions) then you need to figure out a different way. There are about Eleventy Hundred ways to do it.

If you want some advice on how to do it, you'll have to post a basic sketch or segment of the print.

R

Plouch16 said:

Unfortunately the extrusion and saw cut tolerances are +/- .015-.020. So you can see how that variance poses a problem.

Click to expand...

Sure - we can see that.
Not sure why you can't?


------------------------

Think Snow Eh!
Ox

Plouch16 said:

Anybody ever confirm this theory or is it just bs? I have one operator on my Makino a51's that complains about floating edge. We are running common fixtures and AFAIC if the saw cut, and extrusion size is good the concept of a floating edge is irrelevant. I was always taught the 3-2-1 rule for workholding, so I've always perceived that as bulletproof.

Click to expand...

.
.
castings often sit on 3 supports, 2 side stops prevent azimuth (B axis) rotation and 1 side stop prevents it sliding along the 2 side stops.
.
when lengths vary usually there is probing to "stock divide" or center it. so if casting 0.300" big its evenly big .150 on each side so roughing mills have more even load. manually done with a tape measure too but probing a lot faster. stock dividing is a term i never heard of until i worked with big castings. they often vary in size.
.
castings have no good edge. all the edges are floating edges

Getting consistent results with castings or forgings starts with the engineers. The forging drawing should have the 6 tool points defined, and dimensioned from the machine reference planes in each axis. It's the foundry's responsibility to make sure there is a part withing the T.P./MRP space.

The tool point fixture is built off the forging drawing, with a stop or tooling button at each tool point. That locates the forging in 3 axes, with the tooling points as the machine reference location.

First machining operation is done on the tool point fixture and establishes the machine reference planes, from which the part datums are defined. Datum -A- is dimensioned from MRP -A-, etc.

The second fixture locates the part on the MRP's and you have repeatability.

Not many small manufacturers follow this process. Whenever I get castings to machine, I take the casting drawing and start marking it up, putting in my tooling points and machine reference planes so I have a logical way to approach the part.

Plouch16 said:

Unfortunately the extrusion and saw cut tolerances are +/- .015-.020. So you can see how that variance poses a problem.

Click to expand...

This is the perfect way to illustrate, how the stacking of tolerances doesn't just apply to assemblies...

Technically, your extrusions & saw-cuts could all be in tolerance, but if all the tolerances fall on the plus, or minus side, then some other critical dimension - true position of a hole, from one of the exterior edges for example - could be off by a mile.

If you guys are seriously registering against saw-cut edges, and are expecting to hold tight-tolerance to the opposite side of the part, then you're blind, or crazy.

I've machined a lot of irregular forged parts in the past, which went through many operations/fixturings to finish the part. Just like in your example, there's a lot of variation on the incoming parts. You have to plan & anticipate these changes, and fixture the parts to allow for that.

Nerdlinger said:

I think dimensioning off a “floating edge” is fine as long as that surface is qualified during machining...just like you would in a VMC - If Z0. is the top of a saw-cut part you would “qualify” it by face milling to Z0. after ensuring the part is ALWAYS saw cut to at least .001 talker than the finished length.

Click to expand...

I don't mean to single you out, but I can't ignore this. We may be splitting hairs here, but it's important.

You wouldn't dimension from this "floating edge" or sawed surface on a precision part. You dimension from a qualified surface - one that's been machined, or at least good condition from the bar. (If the designer really did dimension from a saw-cut edge, then it's some manner of rough-ass part, that doesn't warrant any discussion on a precision machining forum... )

In your above example, if the top surface is saw cut, and you plan to machine this surface, then Z-zero is not the "top" of some rough sawn surface. It's at a carefully selected distance below where you expect that saw-cut surface to be. That is your datum/Z-work offset/qualified surface.





Maybe I'm in a bad mood today, but I can't believe the OP is having this much trouble understanding how varying stock allowances on incoming parts, can play havoc on tight-tolerance dimensions.

If there's tight-tolerance features that are being lost because of varying stock allowance on one or more edges, then you have to either 1-pre-machine the parts before the critical operation, 2- find every part by touching-off, or probing each part, or 3- change the fixturing to either clamp on a different surface, or compensate for any variations in stock allowance. (IE, use a self-centering device for fixturing - a 3-jaw chuck is a perfect example.)

Jashley73 said:

I don't mean to single you out, but I can't ignore this. We may be splitting hairs here, but it's important.

You wouldn't dimension from this "floating edge" or sawed surface on a precision part. You dimension from a qualified surface - one that's been machined, or at least good condition from the bar. (If the designer really did dimension from a saw-cut edge, then it's some manner of rough-ass part, that doesn't warrant any discussion on a precision machining forum... )

In your above example, if the top surface is saw cut, and you plan to machine this surface, then Z-zero is not the "top" of some rough sawn surface. It's at a carefully selected distance below where you expect that saw-cut surface to be. That is your datum/Z-work offset/qualified surface.

Click to expand...

What you said is what I meant...I just didn’t word it appropriately, but in the name of future helpfulness for anyone referencing this thread - thank you! I suppose I meant to say that if the sides of the part that are clamped against your locators are, for whatever reason, not the same sides that the print dimensions are referenced off of that is okay as long as you qualify those sides in the machining processes.