Sierra "Makin' Chips" video series.

If it has Pedals...
ljs
Posts: 101
Joined: Mon Sep 06, 2010 1:30 pm
Location: North East(the town) PA

Re: Sierra "Makin' Chips" video series.

Post by ljs »

Hi Ross, I just watched your latest video. I was wondering in your programming, the nesting application? Are there parameters to instead of telling it 14 pieces are needed, just to make as many as possible from the piece you have. In the video ( 3:13) where you show the suggested milling pattern seems like possibly 2 more pieces could have been machined. Not that that's a big deal, but I was mostly just wondering if that option is available. Thanks for the videos.
LaVern
Ross Shafer
Posts: 189
Joined: Tue Nov 24, 2009 11:52 am

Re: Sierra "Makin' Chips" video series.

Post by Ross Shafer »

hi LaVerne,

You caught me just before heading out to make some chips. This is new software to me and I'm horrible at learning software. I haven't found what you're asking about, nor have I really looked for it. In the beginning of that part I was actually trying to get 15 or 16 parts from the 1' square, but the software would only place 14. I probably could have gotten another one or two out of it if I'd made my border min distance from part edge to material edge.

Thanks for watching!
dragonworks
Posts: 20
Joined: Sun Dec 10, 2017 3:15 pm

Re: Sierra "Makin' Chips" video series.

Post by dragonworks »

ljs wrote: Fri Dec 15, 2017 11:31 am Hi Ross, I just watched your latest video. I was wondering in your programming, the nesting application? Are there parameters to instead of telling it 14 pieces are needed, just to make as many as possible from the piece you have. In the video ( 3:13) where you show the suggested milling pattern seems like possibly 2 more pieces could have been machined. Not that that's a big deal, but I was mostly just wondering if that option is available. Thanks for the videos.
LaVern
in standard G code on milling machines you make the main program a subprogram, call up another work offset and machine another part.
It would look something like this.
G0 G90 G54 X0 Y0 S30000 M3 (MOVE TO START POSITION OFFSET G54 TURN ON SPINDLE)
M97 P1234 ( CALL AND RUN LOCAL SUBPROGRAM 1234)
G0 G90 G55 X0 Y0 (RETURN FROM SUB, GO TO X0 Y0 OFFSET G55)
M97 P1234 (CALL AND RUN LOCAL SUBPROGRAM 1234)

All the work to do the machining would be in the subprogram which would be program 1234
the holes and the contour would necessitate two separate sub programs.

that is one way of doing it.
you want to run each tool on each offset, if you are using more than one tool, not run the whole part on each offset or you are changing tools to often.

On the mills you can position your spindle anywheres, call a G92 setting a temporary zero and run the whole program as a sub program but then you would be changing tools for each piece. There are ways around that but it gets a little tricky. G92s were replaced by work offsets, on a fanuc it would probably be G54, G55, G56, G57, G58, AND 59 etc.
There are other ways to go about it.

I don't know what software is being used here or what type of code but they should all be able to do about the same thing.
Last edited by dragonworks on Fri Dec 15, 2017 2:22 pm, edited 2 times in total.
dragonworks
Posts: 20
Joined: Sun Dec 10, 2017 3:15 pm

Re: Sierra "Makin' Chips" video series.

Post by dragonworks »

Ross Shafer wrote: Fri Dec 15, 2017 11:07 am Where do you live? You're welcome to come help me anytime!

Just posted another vid, this time I'm making some thin aluminum parts on the router....probably won't do it that way again, but had to check it out. https://youtu.be/2ohNiY6laNA

Have a great weekend and Happy Holidays!!
I live on the east coast but would be glad to be of any help, I am a walking encyclopedia of useless machining facts.
Watching the "aluminum" video I see that you have nesting software. I also see you are helically interpolating the holes.
Will the router drill holes?
I programmed for lasers for 3 years and that had nesting software, made life easy. With the laser software program you could add individual parts, drag parts around,spin them, reorient them. Many times programming parts on 4x8 sheets of metal, the software did not optimize the parts on the sheet, I could add more.
Ross Shafer
Posts: 189
Joined: Tue Nov 24, 2009 11:52 am

Re: Sierra "Makin' Chips" video series.

Post by Ross Shafer »

Hi Jerry,

East coast eh? Dang, I could learn a ton from you! Lemme know when you want a nor cal vacation, maybe we can work something out.
Ross Shafer
Posts: 189
Joined: Tue Nov 24, 2009 11:52 am

Re: Sierra "Makin' Chips" video series.

Post by Ross Shafer »

I hope everyone had a wonderful Christmas and that the New year will be a good one!

We just posted another video, this time I'm making the changer stop bar/return spring mount.

Thanks for watching!
dragonworks
Posts: 20
Joined: Sun Dec 10, 2017 3:15 pm

Re: Sierra "Makin' Chips" video series.

Post by dragonworks »

watched the finger stops, looks like your speed and feeds are pretty good. Is the video real time? Are you using carbide endmills? How many flutes?
Ross Shafer
Posts: 189
Joined: Tue Nov 24, 2009 11:52 am

Re: Sierra "Makin' Chips" video series.

Post by Ross Shafer »

Hi Jerry,

Most of the vids are sped up by some amount...not nec. consistent from vid to vid. I do use Carbide 2 flute as much as possible, but still have quite a few HSS cutters in the mix. I'm flying by the seat of my pants with most of my feeds and speeds the numbers kicked out by MCAM seem more suited to a bridgeport, so I always put in my own numbers with an eye on chip load....the vast majority of stuff I do is in aluminum which seems to be pretty forgiving.

There's nothing I'm doing in quantities that require making the stuff as fast as possible. I'm sure that's obvious to you with some of the programming you'll see in those vids.
dragonworks
Posts: 20
Joined: Sun Dec 10, 2017 3:15 pm

Re: Sierra "Makin' Chips" video series.

Post by dragonworks »

For anyone who needs the info.


speeds and feeds. First I have to have a starting point on metal removal,= surface feet.
For carbide, Aluminum surface feet should be somewhere between 1000 and 1500
for CRS about 350-500
RPM= surface feet x 3.82 / by cutter diameter.
example three flute 1/2 carbide endmill in aluminum

(1000sfm x 3.82) / .5= 7640 RPM
I usually run the 1/2 inchers (three flute) at 7450rpm at 50 inches per minute, no problem

for feed rate you would go by inch per tooth= (feed rate / rmp) / number of teeth

in the above case that would be (50ipm / 7450 rpm) / 3- number of teeth = .0022 per tooth witch is a light cut
a heavy cut would be .010 per tooth.
light cut up to .005 per tooth, heavy cut .005 or more per tooth.

I guess I should up my speed and feed a bit? Depends on depth of cut also. But those two formulas, as long as you know the surface feet of the material you are working with, and the cutter material, should get you in the ballpark. You can make your own library in Mastercam if you want. I did because I don't know who set the libraries up in the MC version I am using but some of them are absolutely out of the question. If your cutter gets small enough mastercam will spit out spindle speeds way faster than your machine can do. Going to slow with RPM or IPM can cause the tool to "rub" and wear out prematurely.

The machine also needs the horsepower to do the work, that is another formula but I never really have to deal with it, although I have. We have a 25 horse machine at work, but I had to explain to my bosses why it keeps stalling out trying to deck .1 on a piece of A2 tool steel. With a 6 inch face mill you can only do about 150 RPM (250sfm x3.82) / 6 = 159). At 150 RPM the machine only delivers about 4 horsepower and stalls out. I had to put the bosses on the phone with HAAS and so they could get it from the horses mouth.
Ross Shafer
Posts: 189
Joined: Tue Nov 24, 2009 11:52 am

Re: Sierra "Makin' Chips" video series.

Post by Ross Shafer »

Unfortunately my mill only goes up to 6k rpm so most of what the math gives me won't fly on my machine with aluminum (95% of what I cut on it), so I wing it from there.

My Mcam spits out ridiculously low numbers for everything it seems....I too have my own library going.....kind of.
Post Reply