Feeding in to position

[BBprecise]

Me and some of the operators are having a conflict. We don't agree on which way to feed in to direction when machining a hole that requires us to feed in to position to achieve the positional tolerance. I have always fed in the X+, Y- direction at the same time, another operator feeds in the X+, Y+ independently, and another says there is an industry standard to feed X-, Y-. What do you all do?

[spade117]

Usually, whatever mastercam spits out.

[RandleXX]

Usually, whatever mastercam spits out.

 

^^^ Yep.

[K2csq7]

Tight positional tolerance (tighter than machine can normally hold), I will send the machine home (x &y) then move to position with an indicator, verify the numbers are correct (adjust offsets and repeat until position is good) and then make the same moves for machining (from home position to location).

[GoetzInd]

I don't think it matters as long as it is approached the same direction on each feature for maximum repeatability. Our makinos have a option that automatically does this. Never used it though.

 

Mike

[Dave.L]

This is all related to backlash in the ball screws. If you are having issues, you may need a minor service call to adjust the comp settings. If you are doing drill/ream/bore positioning, many machines have a code called "one way positioning" which will always approch the final location from the same direction to take up the backlash. I have our posts setup to do this.

[Allan]

I agree with the "One way Positioning" I seen this on many machines, "M60" comes to mind.

In my opinion if you need to do something like this then you either have something wrong with your machine (backlash or worn out thrust bearings), or the tolerancing is too tight for the process and should probably be done on a jig bore.

 

Allan

[Mr. Wizzard]

I'm with Allan and Dave. It shouldn't matter unless you have way too much slop in the machine or are trying to make something tighter than the machine was designed to accomplish.

[BBprecise]

We do this when we have to hold a true position of .004 or less. Sometimes it's in relationship to a datum surface we're locating on, but usually it's from one hole to another that are being machined at the same time. The mills are Fadals and maintenance is a running joke around here (we adjust the backlash ourselves, one machine has .004 on the Y axis in the center of the travel). You don't want to know what happens when you put an indicator on the table at one end of the X travel and move to the other end. A lot of our parts have .002 true position and even the machines when they were new would struggle to rapid into place and hold .003 true position so we do what we can with what we have. My theory is as long as you do it the same way it doesn't matter. I just kind of laughed though when one engineer said there's an industry standard when it comes to this.

[Allan]

BBprecise, with all respect, I highly doubt that you have .004 of backlash (ball screw wear), the setup on a Fadal uses a set of opposed tapered thrust bearings these are most likely worn out.

The bearings will run you about $80.00 and maby 2hours to install.

 

 

Allan

[Goldorak]

usually (read always) ,i rapid to position then drill , All our Okuma machines can easily hold a position within .0002 even the 22 year old VR-40

[AshM]

I used to program and operate a old zayer bedmill with a 3 metre (9foot) by 1.2 metre (4foot) table. It was an old machine that had been refurbed with a xxxxor controller on it.... anyway I used to constantly adjust the axis backlash compensation between parts to maintain the accuracy when switching directions. In the mornings the comp could be up to 0.5mm (0.020") and then I would decrease that as the machine warmed up and lubrication got into the slides.... It was truely the most frustrating thing at the time but in hindsight its kind of funny in a way...

 

in fairness to the machine, our workshop would range from -5 degrees C mornings to +25 deg. C mid afternoon (I have no idea what that is in deg. F). And after all of that the machine was still good for +- 0.1 at the worst in a straight line.

[CJep]

BB,

The Fadals use a function in the canned drill cycles called positive approach M46 that allows the machine to go beyond the position by .005 - .030 then "backup" to the position taking out the backlash like manually positioning on a knee mill.

 

Could that be what the operator is talking about?

[Dave.L]

BB,

The Fadals use a function in the canned drill cycles called positive approach M46 that allows the machine to go beyond the position by .005 - .030 then "backup" to the position taking out the backlash like manually positioning on a knee mill.

 

Could that be what the operator is talking about?

 

 

That is only for point to point moves like I stated with "one way positioning" it's the same thing. But, I said this for reference since I think he is talking about circle milling etc..

[GoetzInd]

If you have .004 of backlash, you need to pop the way covers off and take a look. Like others have said, I think support bearings are to blame. .004 is unacceptable, even for a Fadal.

 

Mike

[EX-wccprogrammer]

This is indeed called 'Positive Approach', and I use it for accurate positioning on bored holes.

 

That being said, I always use X+ Y+ so my machine operators understand WHY it is called 'Positive Approach'.

 

Not that it matters which direction you use, as long as you are consistent throughout the program.

[Guest CNC Apps Guy 1]

Me and some of the operators are having a conflict. We don't agree on which way to feed in to direction when machining a hole that requires us to feed in to position to achieve the positional tolerance. I have always fed in the X+, Y- direction at the same time, another operator feeds in the X+, Y+ independently, and another says there is an industry standard to feed X-, Y-. What do you all do?

 

Industry Standard huh??? :headscratch: I don't think so. I'd say "...I'm from Missouri, SHOW ME!"

 

When I need to do it really is a decision I base on a few criteria, age of the machine, backlash error, has the machine been crashed, and what the tolerance is.

[BBprecise]

Allen, as you said I'm sure it's not all in the ballscrews some of it's in the tapered bearings, but getting the scheduler to give us the time to investigate is a challenge so we just use the backlash as a way to keep going. It's pretty bad when I was down there the other day when an operator was indicating a bore in to set his offset and he grabbed the end of the table, gave it a little yank and the indicator showed .001 movement. The owners moto is "If it still moves it ain't broke".

 

 

Goldorak, .0002 at full rapid, must be nice, I've seen 5 new Fadals come through here over 15 years (latest one with Fanuc control) and I don't think any of them could hold that when new and feeding into position (ya get what ya pay for).

 

I'll look in to the M46, I knew about the G60 for Fanuc controls, but don't remember the M46 in the Fadal books.

 

Works slowing a little, so I'm gonna suggest a little PM to save some aggravation. These machines are great for what we used to do, but not with the stuff we do now. Just not designed for it.