Feed rate

[STEELTHOM62]

Is there any way to get MC to use feed per rev

instead of inches per minute? I've tried changing the defaults for commonly used tools but they post out to a feedrate of zero.

As of right now, I change all of my feeds in the editor, but this can get pretty time

consuming.Running V9.0 SP1. Thanks

[kccadcam]

Are we talking Mill or Lathe?

[STEELTHOM62]

Mill

[Roger Martin from CNC Software]

Your feeds will post out as zero because of the output formatting assigned to the feedrate. Mill posts are setup for IPM feed mode (probably 1 or 2 digits to the right of the decimal). You plug in a feedrate of .005 IPR and the output in the NC file will be ZERO. If you cannot handle changing the formatting (It is not very difficult), contact your dealer. One important thing is - are you running ALL toolpaths in IPR mode? If you run milling paths in IPM and drilling in IPR the post work is more involved.

[STEELTHOM62]

I generally run all of my tools and operations in IPR.We run alot of indexable tools and I've always liked IPR better for controlling chip load for each tooth.

[chris m]

If you get your post changed, don't forget to make sure it posts a G95 as .032 IPM is VERY slow

 

Not that I've done that...

[STEELTHOM62]

My machine goes to G95 as a default at start-up.But I have learned a couple of times that 10.0 IPR is very, very, fast.

 

[chris m]

Ouch!!!!

 

That's probably enough to twist the feedrate override right off of the machine!

 

C

[STEELTHOM62]

Luckily,I've got quick fingers on the ol' feed hold button.

[Michael Reynolds]

I'm sure I'm missing something, but why would IPR be used on a mill, outside of mabye tapping??

 

Respectfully,

 

Mike R.

[kccadcam]

Mike,

Just a different way of looking at things,

Inches per Rev - or - Revs per Inch!

Simple calculations to convert one or the other.

 

Lets take a poll:

Most mill guys use inches per minute, Right?

And I would say lathe guys are more inclined to use inches per rev.

Now how about the guys that do both???

 

Just curious........

[Hugh.Venables]

To get IPM first you must have IPR and multiply by RPM. Why bother to do that if you can work with IPR? Once you get used to it I would think IPR would be more useful to read at the machin.. IPM only means something in conjunction with RPM. IPR relates to chip load only via no of teeth. IPM relates to chip load via no of teeth and RPM. But for all that when I enquired about working in G95 instead of G94 I was told "forget it, no-one does it". So neither do I, much as I'd like to.

But back to Kevin's poll. Why use inches when you can use m.m.?

Hugh Venables.

[Michael Reynolds]

Thanks Kevin!

 

I'm just wondering why someone on a VMC would use inches per rev.....? Mayhaps they are lathe people at heart?

 

Very Respectfully,

 

Mike R.

[Guest CNC Apps Guy 1]

I did it one time just for kicks. It was fun to see the expression on their faces. What a sicko I am.

[chris m]

IPR on a milling machine can be nice [especially when proving out a program] if you are not an octopus; if you are fairly confident about your programmed tooth load you don't need to balance your elbow on the feed hold while turning both the feed override and the spindle override to maintain you IPT. I have seen more than one endmill get blown up when the setup guy chops the RPM way down to kill some vibration and the machine keeps feeding away at 2 or 3 times the intended tooth load. It can be a real bitch to get all that carbide out of your part

 

Do you big-time mill guys [which I am definitely NOT as 75% of our work is turning] program drills, taps, and reamers in IPM? Why go through the aggravation of converting your drill feeds since I'm sure most people "think" in IPR for drills?

 

Hugh, you have to give up on this metric system thing, it ain't gonna happen

 

[ 08-29-2002, 07:21 AM: Message edited by: chris m ]

[STEELTHOM62]

I program in IPR mainly due to the fact that that's how I learned to program on my first CNC job.When I started with my current shop I learned to program a Mazatrol M2 control that also uses IPR, I guess I'm just more comfortable with it and I feel like I have more 'control' of the tool.

99% of my work is mill.

 

[ 08-29-2002, 07:42 AM: Message edited by: STEELTHOM62 ]

[Hugh.Venables]

Ah! Chris. That's what all the old cooters used to say over here in the 1960s. Don't fret. It'll happen.

 

Steelthom62 I agree 100% with you. IPR is a stand alone dimension. IPM is meaningless without RPM. Also as you said the machine will maintain tooth load with IPR if the operator overides the RPM at the machine and IPM won't. I can't see any reason for using IPM. Only problem is you're right and everyone else (almost) is wrong/different which can lead to confusion.

 

Hugh Venables. (supporter of lost causes)

[Jack Mitchell]

The argument of inches per rev over inches per minute has been a bone of contention with me ever since I learned Mastercam ver 4.

I guess it all goes back to using a water wheel in a stream or the like.

 

Conventional milling machines used a power take off from the main motor. These power take-offs revolved a one specific rpm. To get different feeds the machine tool builder needed to incorporate gears & levers in order to gain the different inches per minute that they needed to perform effective cutting based on the rpm of the motor. All of this was in the 30s, 40s & 50s. – Inches per minute was based upon the rpm of the specific machine tool motor.

 

The older journeyman or toolmakers simply observe a cutting process and say bump it up, slow it down, increase the rpm, increase the feed, etc!, these guys have been around for ever. Chances are they would balk at the newer technology of chiploads & depth of cuts. However; when viewing a 2” Facemill at .105/rev is an incredible sight = 325”/min. - I do not know of a machinist that can turn the handwheel at that speed; or even half of this.

 

We, the newer generation, have been shown or taught of optimum cutting conditions etc!

Personally, it wasn’t until I experienced Mazak machine tools that I actually learned what I know today. (Actually, I am looking forward to abusing a 1.25 diameter 390 Coromat – 17mm insert, with the salesman’s blessing- I will beat this cutter to a pulp, and the salesman will thank me ever inch of the way – of course, he will also want the video tape – and WE are going to get it here FIRST, on this forum.

 

In a nutshell; program your feeds using G95 this will make you more knowledgeable with cutting conditions.

OR

Do it the old fashioned way use (G94) and add another step by multiplying the rpm by the feed.

 

The largest benefit of using G95 – is that if you bump the spindle speed by 30%~ the feedrate will always remain constant and maintain its chipload..

If you choose to use G94 – bump up your spindle 30% + you also have to override the feedrate by 30% - adjust one or try to adjust both overrides- you decide.

 

One other benefit is that you can actually do a restart & tap a hole as many times as you want – this will always synchronize when using G95.

 

One other point; I believe an encoder is required right next to the spindle (this will count the actual revs) hence the difference between synchronous & asynchronous (SP) feeds.

 

Glenn Bouman at In-House Solutions will vouch that I have indeed brought this up with him many, many times. I cannot change the habits of those who will not progress. I can however challenge the Cnc Software to make a positive step and default Mastercam to units per revolution – this made perfect sense 20 years ago, let’s be a first here and break this vicious cycle.

 

Regards, Jack

[MetalMarvels]

It would be nice to program in IPR since the mill tools are generally specified that way, but my VMC will not accept a G95 - only a G94 so the direct IPR method is not available to me.

 

Thanks for the history.. I have always wondered how some rather strange ways of doing things have come down to us.

 

Regards

[Jack Mitchell]

Metal Marvels,

 

That's the part I cannot figure. Why would we ever choose G94 over G95?

Basically, 50% of all Cnc machining centers are still programmed using G94.

Why still do those shops that use this archaic code still endorse this?

Old habits do indeed die hard.

Kill the G94; G94 must die!

 

Regards, Jack

[Hugh.Venables]

Crikey Jack, just as I'd written you off as Multax re-incarnated you come up with some good stuff.

 

Many conventional machines had separate spindle and feed motors with no chance of synchronous feed hence IPM on the feed gearboxes. I think we should flog the point a bit harder that G94 is a left over of these steam powered machines and there is no longer any need for it. It's just there for some people's old fashioned comfort zone.

Older CNCs didn't have encoders. The control "knows" within reason what the spindle and axes are doing and is able to synchronize the feed. It comes a bit unstuck on tapping, particularly on reversal where it has no idea about over-run. For this we need floating tapping holders. Machines with encoders always know exactly where the spindle and axes are allowing rigid tapping.

 

I'd be wary of restarting a tap in a tapped hole, I suspect only machines with encoders will do this successfully.

 

Gary, are you absolutely sure your control won't accept G95? Surprising.

 

Hugh Venables. (maybe this ones not a lost cause after all)

[chris m]

quote:

---

Gary, are you absolutely sure your control won't accept G95? Surprising.

---

Believe it. I have a couple [old] machines that won't accept G95. I have a feeling that it may be an option we didn't buy at the time (we didn't even buy man-readables if you can believe it) but they don't take it. This, of course, drives me nuts as I like to program this way; it's always nice to look at the block data in the control while its running and have a good idea of what the machine is doing without breaking out the calculator. Now, if I could only program surface footage instead of RPM...

 

[ 08-30-2002, 07:14 AM: Message edited by: chris m ]

[k_barry]

Yes I agree that units per rev are far better than units per min.

If I reduce the spindle override by 30% I dont want the feed to increase.

I think units per min were an old hangover when we had manual milling machines with separate drive motors working independantly.

I changed over when using an old VMC which took a long time to start the spindle. If I started the spindle close to the job it would run into the job before the spindle started!

 

But haven't we got away from the original question, or have I missed it. Can Mastercam do units per rev on a VMC (all the time will do me)

I only want units per min when the spindle is stationary.

 

My old CAM system had the option, both for the lathe and mill.

 

Regards

[MetalMarvels]

After reading the ensuing responses, I went back to confirm that my VMC will not accept a G95. After checking with my dealer, I have confirmed that my 2000 vintage VMC will not accept a G95 - a little surprising since I can Rigid-Tap and I can re-enter a tapped hole as many times as I want without buggering up the tapping (as long as I start from the same z-height every time of course). My VMC is one of the entry-level systems however and a G95 just wasn't included....

 

Cheers.

[Flycut]

So...

After 10 years (last time someone posted in this topic) is there a way to use G95 for all milling in mastercam?