Max spindle speed and related feed rate adjustment...

[?Mark]

Finally have some free time to continue setting up my tool libraries and I'm wondering how everybody is working around this issue:

Lets say I pull a 1/16 endmill from my library for which default rpm is set at S21401 and feedrate at F40.0 ipm.

 

When posting, rpm is adjusted to the maximum allowed by a machine in general machine parameters but feedrate is not scaled down accordingly so in some cases it can result with an .0625 mill doing S6000 and F40.0. Now that WILL brake a tool

 

Is there a way (post or elsewhere) to have mc scale down a feedrate proportionally to where the rpm was scaled?

In this case S21401/6000(max rpm)= 3.5668 (scale factor)

and F40.0/3.5668= 11.21 (correct feedrate)

 

Any ideas?

 

Regards, Mark

[crazy^millman]

Well I could create machine tool libraries based off of what the machine can do and have my speeds and feeds done in that fashion verses using material libraries to assign speeds and feeds which would cause the problems you are seeing.

 

HTH

[Tim Johnson]

If you have different libraries are setup for each material then yes you can. What I did is set up a generic material in the material manager called "All Materials". Everything in there is setup at 1000 sfm and .010 fpt. Then in the tool manager I set (still setting) the material cutting speed %/material feed per tooth% for each individual tool based on the material the library is for. Also make sure your number of flutes are correct. There's a lot of effort to do this but very well worth it in the end.

 

Note: you can use the preset library materials but I fould them to be too generic for me.

[?Mark]

quote:

---

create machine tool libraries based off of what the machine can do

---

There has got to be a better way

quote:

---

There's a lot of effort to do this but very well worth it in the end.

---

Again, there has got to be a better way

 

Basically, I'm trying very hard to stay away from material libraries or creating multiple tool libraries based on specific machine...

 

Thanks guys, and please keep suggestions coming...

[Guest]

It's off the wall at least from my perspective but how about running your machine in G95 and setting all of the tools to IPT instead of IPM.

 

Then at least as you adjust spindle speed you'll adjust feedrate.

 

Just throwing it out here to see if it sticks

 

Actually I am just being a post xxxxe.

 

[?Mark]

It works well on a lathe but it would be great to get this as easy on a mill, don't you agree?

[crazy^millman]

It is that easy on a mill you just use the correct G-code and all most any mill will work in feed per rev. Problems is most people think of that as a crazy concept where as if more people did it they would get back to what I call the basics of machining where chip load per tooth is more important that feed per inch is IMHO. If you have ever run a Mazak then this concept is 2nd nature to you.

 

If you want to make a post do it it can be done just requires the right logic in the post you need to probaly look to the MPMASTER post and use some of the tool information to control this then you would want to create a material logic in which you drive them from as well as a machine logic to pull the information out of the machine definition so that if you post with a certain machine with a limited spindle speed it will then use the above material and tool information like length of flute, number of flutes and material you are cutting with like highspeed or carbide as the SFM calculator for all of the needed caluclations. Now all you have to do is make sure that you describe all of your tool 100% correct in your library, then make sure everytime you send a program to the floor they use that same each tool 100% of the time and all should be good. I figure probaly couple 100 lines of added post code for the logic should do what you are looking for.

 

Yeah I think that would be a lot easier than using machine speific libraries.

[?Mark]

Ipr is not a new concept to me, but would like to avoid it on a mill.

So in a nutshell, nobody has figured a way around it yet, at least not without using material AND tool libraries?

imvho, scaling down rpm without taking a feedrate into consideration is a "butcher" way of doing it. I think it could use a little TLC from CNC...

Pretty please

 

Regards, Mark

[crazy^millman]

Sorry was not trying to Imply you did it was just a way in which you could do it. Are you a Beta tester? If so look on the Beta Forum there is something there you might be able to use. Email me and I will explain.

[Psychomill]

Mark, Yes you can scale feed. I've been doing that in posts for quite a few versions now. All you need to do is create a formula for the math, a variable for MC to use, and the calculation for the feed to use. Something like this: (note: this is from a converted post that I've been using since V7)

 

First, create a string to save the current or programmed spindle speed... like "savess" or something. Then, you just create the math:

 

pfr # this will scale the feedrate if the max rpm is excceded

scalefr = savess / ssmax

if savess > ssmax, fr = fr / scalefr

if fr > 0, fr

 

For MCX built posts, I think the variable is "maxss". I'm not near a X post right now to check this. Anyway, hope you get the idea... This is coming off the top of my head so bear with me. You can also create a safety line for negative outputs in case the scaling brings the feed to less than "0" to have the post give you an error while posting or a command line in the program that the machine won't run. Gotta get moving... things to do... I'll check back later if you've got questions....

 

 

 

Edit: Call Mark over at Triad (if he's still there). I think he knows how this is done as well... If not, I'll check back

[Tim Johnson]

quote:

---

So in a nutshell, nobody has figured a way around it yet, at least not without using material AND tool libraries?

---

The way I look at it is you will get out of your libraries what you (or someone else) put into it. If you do nothing then in a year or so you'll still be adjusting feeds and moaning about it while I just click on a tool and go on my merry way.

 

Edit: Psychomill has saved the day...

[?Mark]

Ron, mail.

Rob, I'll do.

Tim, you got me wrong here I think. I know tool libraries are a lot of work that MUST be done correctly, I'm just trying to avoid creating separate for different machine tools.

The way Rob has it setup (I think) is that no matter what machine you have active (whatever the max rpm) the chip load will be the same when mc scales down the rpm, and thats what I'm after here.

 

quote:

---

The way I look at it is you will get out of your libraries what you (or someone else) put into it

---

+1

I couldn't agree more Tim.

 

[Tim Johnson]

Mark,

 

I have one library for one material that all the machines use. I just have around twenty materials which means twenty libraries. The reason why I started using the speed/feed %'s was to eliminate the extra libraries and not having to re-edit the tools everytime we get a higher rpm machine.

 

Yeah, Rob's way does look a lot easier to set up. The only issue I see with that is lying to the machine defs about the minimum/maximum speeds and that's not a big deal. (I'm imagining the looks on our operators when they see 48000 rpm on the tooling sheets for the Fadals)

[?Mark]

LMAO. Yeah, I could see a panic in their eyes already.

I just checked on my setup sheet and it shows the adjusted max rpm instead of the the one from the tool library, so all should be well me thinks...

[Psychomill]

note:... I'm setting up a new part on a FH8800 so bear with me here....

 

 

quote:

---

The way Rob has it setup (I think) is that no matter what machine you have active (whatever the max rpm) the chip load will be the same when mc scales down the rpm, and thats what I'm after here.

---

Yes, thats the way it works. It maintains the chip load no matter what rpm. And it works both ways, whether you go up or down. Although going up has other issues since you have to edit the running rpm for the tool parameter which will try to draw the chip load setting from the material/tool library. At one shop, we used to just program to the highest speed spindle we had. Then it didn't matter for which machine we posted... it was at least the same rpm or less which the post took care of. I don't bother with material libraries and tool libraries are only set for max conditions and tool matrix on dedicated machines.

 

quote:

---

The only issue I see with that is lying to the machine defs about the minimum/maximum speeds and that's not a big deal. (I'm imagining the looks on our operators when they see 48000 rpm on the tooling sheets for the Fadals)

---

You don't have to lie about machine definitions.... at least you shouldn't. The beauty of this post is that you can just simply change the post to have an adjusted program for a slower machine. No need to mass edit common parameters within the operations manager.

 

Now I don't know how this will affect your tool sheets since I don't use MC's tool sheets either (Don't like it... ). But looks like Mark says it works....

[Psychomill]

Edit....

 

"And it works both ways, whether you go up or down." This is miss-stated somewhat. Going "up" was another post that had a script prompt to change RPM by a percentage and thereby changing the feed. Didn't use it much.... only scaled down mostly which is easily handled by the post....

 

Bedtime... more setting up tomorrow....

[?Mark]

Went to the Denver Machine Tool Show yesterday and to my surprise there was a Mastercam booth.

I had a pleasure of meeting Doug Nemeth from CNC Software. Together with my reseller Mark we talked about this subject (scaling feedrate) and hopefully he can get something rolling soon.

I got busy again today so I didn't have much of a time to play with it, and I know just barely enough to be dangerous

Mark also mentioned that he's done it in the past so my hopes are high.

Anyhow, I'll keep you posted if we get this figured out.

Thanks for your help Rob and others

[Henk]

I'm in the same process.

i,ve now 12 different tooltable's for the Mat.groups we use

For 2 machine's that would bee 24

 

I like Psycho's way, but i would add some things.

To save the spindle i will not allow all tools to go to the max. Some thing like:

1mm and under tools, max 100%

1.5 - 3mm, max 95%

3mm and over, max 90%

 

An minus for this is that it infect the given machine time in backplot.

[?Mark]

quote:

---

An minus for this is that it infect the given machine time in backplot.

---

+1

Backplot is not very exact at this time, but you're right, it'd be very nice if feedrate scaling could happen BEFORE posting.

[Henk]

quote:

---

it'd be very nice if feedrate scaling could happen BEFORE posting.

---

When it's done in the post, it is easyer to switch between machines.

 

An other thing i'm planning is 'fixed toolnumbers' for all tools.

Our heidenhain controls can have over 30000 tools in their tool-table, the place-table tells the control which tools are in the chain and where.

[?Mark]

I think a little check mark in machine def or control def would do the job quite nicely...

but I'm getting a little ahead of myself here

[Psychomill]

quote:

---

1mm and under tools, max 100%

1.5 - 3mm, max 95%

3mm and over, max 90%

---

You can have the post calculate for this as well based on the tool used. Just have to stipulate tooltype and diameter to the equation.

 

quote:

---

nice if feedrate scaling could happen BEFORE posting.

---

I think it can, but its going to take a tool/material library thats set up for the machine in question to do this. I'm guessing you'd end up having to edit common parameters from the "current tools" page of the NC utilities. Bad part might be is all the regenerating.

 

quote:

---

An other thing i'm planning is 'fixed toolnumbers' for all tools.

---

Wouldn't this be a "Tool Library"??

 

[Jeremy Grigsby]

What is bad about IPT? It is much easier on the tools than a programmer just punching in what IPM they think is good for the tool. I don't program mills anymore, only the lathe, but if I would have known about posting sfpm and ipt i would have definitely done that. I for the most part used the manufacturers recommended IPT and SFPM and calculated rpm and ipm. I second a comment about the mazak. It was great on that machine as you could always see what ipt you were running. Sure were going to push it faster than recommended alot of times. I exceeded recommendation quite a bit. I don't know where I'm going with all of this. I just wanted to hear the reasoning for calling IPT a bad idea.

[tryon]

Funny how we will complain about a few extra mouse clicks, but we will guess at IPM or convert IPR and SFM to IPM all day long.

 

Time for a paradigm shift people

[Psychomill]

LOL!!! Touché tryon....

 

There many valid reasons to do either and it can be debated for a long time. I see it though from a "general public" or common point of view. Feed the ego per se.... Coming from a mill, its much more "impressive" to say that you're feeding at 1280 IPM than to say .040 IPT.... To a lathe guy it might not make much sense unless he's telling someone he's moving at .08 per rev...