Hello Guest it is October 17, 2019, 09:40:41 AM

Author Topic: To Ramp, Or Not To Ramp. That Is the Question.... And Others...  (Read 7189 times)

0 Members and 1 Guest are viewing this topic.

To Ramp, Or Not To Ramp. That Is the Question.... And Others...
« on: October 16, 2008, 04:47:46 PM »
1) I'm using SheetCAM to generate G-code for my mill.  I've just gotten the Z axis CNC'd, so I'm learning how to program in 3D now.  SheetCAM supports ramping, but I'm not real clear on when this is advantageous, as opposed to just plunging in Z, then moving in X/Y.  Ramping is kinda fun to watch, but slows things down quite a bit.
So, when/where/why should I ramp.

2) When drilling aluminum (6061), I usually end up with huge masses of "strings" wrapped around the bit.  How do I prevent this?  I'm generally "pecking" 1/8-1/4", but even that is enough to generate a huge quantity of "aluminum wool".

3) When cutting, for example, the perimeter of a part, I usually end up with a small "divot" in the profile at the start/end point, even when I arc in and out.  I do have a small amount of backlash (under 0.001"), but this seems like more than that.  How can I avoid this?  Am I not doing the best kind of entry/exit?

Regards,
Ray L.
Regards,
Ray L.

Offline Hood

*
  •  25,855 25,855
  • Carnoustie, Scotland
    • View Profile
Re: To Ramp, Or Not To Ramp. That Is the Question.... And Others...
« Reply #1 on: October 16, 2008, 04:58:46 PM »
1. ramping is used especially when you have an endmill as they are not centre cutting and therfore cant plunge in. Yes I know you get centre cutting endmills but are they really endmills or just 3 and 4 flute slot drill ;)

2. Alu, especially the softer grades are a PITA and possibly faster feeds may help.

3. Probably spindle deflection, I get this on the Bridgeport, partly  because there is some wear in the bearings but mainly because Bridgeports are about as rigid as a  piece of string ;D

Hood
Re: To Ramp, Or Not To Ramp. That Is the Question.... And Others...
« Reply #2 on: October 16, 2008, 08:53:46 PM »
1. ramping is used especially when you have an endmill as they are not centre cutting and therfore cant plunge in. Yes I know you get centre cutting endmills but are they really endmills or just 3 and 4 flute slot drill ;)

2. Alu, especially the softer grades are a PITA and possibly faster feeds may help.

3. Probably spindle deflection, I get this on the Bridgeport, partly because there is some wear in the bearings but mainly because Bridgeports are about as rigid as a piece of string ;D

Hood

Hood,

1) So, if I have center-cutting mills (which are the only kind I buy....), then there's no reason to ramp?

2) I'll give that a try - maybe faster feed, shorter peck?

3) You know I don't want to hear that!  :-)

Regards,
Ray L.
Regards,
Ray L.
Re: To Ramp, Or Not To Ramp. That Is the Question.... And Others...
« Reply #3 on: October 16, 2008, 10:49:32 PM »
Ray,

Plunge end milling requires slower feed down. It wants to jump around, not like a drill with a center.
 Ramping works better,because you can use more feed then plunging. so your not really losing that much time.
Ramping can also be set to a specified ramp angle. I personally prefer ramping over plunge.

Drilling alum, use a shorter peck,possibly more feed. I hate when that happens.(stringing chips flying around and tearing off coolant lines ,
 Spraying coolant all over my couch.)  :D  It's hard to get away from.


  Ray, Arcing in and out of a linear move should leave no divot. I've use this procedure for milling Ferrari trim 78" long.
when I have to move the piece and continue.
Are you climb cutting?

Ed
Ed VanEss

Offline Sam

*
  • *
  •  988 988
    • View Profile
    • hillbillyhilton.com
Re: To Ramp, Or Not To Ramp. That Is the Question.... And Others...
« Reply #4 on: October 17, 2008, 12:32:39 AM »
Quote
I usually end up with huge masses of "strings" wrapped around the bit.  How do I prevent this? I'm generally "pecking" 1/8-1/4"
That's a heck of a peck. What size drill are you using? What RPM? Usually the larger the drill, the slower the rpm, the more peck distance you can get by with. Obviously, a small bit at 1200 rpm+ can make a stringer chip in an instant, therefore needing a small peck distance. Couple the small peck distance with the addition of a higher feed rate, and you will reach the peck sooner, thus decreasing the chip length even more.
I hate stringers. They are dangerous, and I usually end up getting cut with them. Either from cleaning them away from the tool, or cleaning them up from the machine, or having to pull them out of the broom.

Quote
I usually end up with a small "divot" in the profile at the start/end point
Are you doing a finish pass? How many? how much material are you taking in the finish pass? How thick is the part? What's the endmill size? RPM?
You definitely need to take finish passes. Pretty much all machines have some amount of spindle deflection. Even if it didn't have any at all, endmills flex. Allot more than one would normally think. The larger the endmill, the less the flex. Personally, I like doing finish passes in aluminum with a sharp, smaller endmill at a very high RPM, and a bit faster feed, with lots of coolant to keep the chips away to avoid pulling them back through the cutter again. The high feed also tends to smooth out everything such as ramps and turns and such. On the old worn out machine I use it does anyhow!

Remember to use an oil based coolant with aluminum. Kool mist or other type coolant just won't work well at all. WD40 in a spray bottle is better than nothing.
"CONFIDENCE: it's the feeling you experience before you fully understand the situation."

Offline Sam

*
  • *
  •  988 988
    • View Profile
    • hillbillyhilton.com
Re: To Ramp, Or Not To Ramp. That Is the Question.... And Others...
« Reply #5 on: October 17, 2008, 12:43:23 AM »
I have never used sheetcam, but I would suspect that you could start and end the cutting points anywhere you want. If it's possible to start and end the cuts at corners, or some other feature, the ramping divots may become less pronounced. If a good finish is desired, that's generally what I try to do, anyhow.
"CONFIDENCE: it's the feeling you experience before you fully understand the situation."

Offline Hood

*
  •  25,855 25,855
  • Carnoustie, Scotland
    • View Profile
Re: To Ramp, Or Not To Ramp. That Is the Question.... And Others...
« Reply #6 on: October 17, 2008, 02:26:41 AM »
Oh another thing about ramping is you will tend to chip the material rather than getting streamers which you will with plunging.

Hood

Offline jimpinder

*
  •  1,233 1,233
  • Wakefield, West Yorks, UK
    • View Profile
Re: To Ramp, Or Not To Ramp. That Is the Question.... And Others...
« Reply #7 on: October 17, 2008, 08:53:20 AM »
I know **** all about this - but surely, if you are plunging into a piece, and making metal streamers, then if you look at the work side on, you must be describing a spiral with the cutting edge. I have the same problem with the lathe - the last lot whipped round my chuck and took out my limit switch wiring.

If you increase the speed of rotation, and decrease the feed slightly, then the cutting edge with not bear on enough metal to make a streamer, or it will be so thin as to break apart.
Not me driving the engine - I'm better looking.

Offline Hood

*
  •  25,855 25,855
  • Carnoustie, Scotland
    • View Profile
Re: To Ramp, Or Not To Ramp. That Is the Question.... And Others...
« Reply #8 on: October 17, 2008, 09:26:24 AM »
Jim, probably the way to stop this happening on the lathe is deeper cut and faster feed for a given spindle RPM. This is assuming you are using indexable insert tooling as they have built in chip breakers. Your machine may not have the power to take advantage of this however but here is a pic of the chips in the lathes swarf tray. Not saying I always get nice wee curly chips but I am getting better :)

Hood

Offline jimpinder

*
  •  1,233 1,233
  • Wakefield, West Yorks, UK
    • View Profile
Re: To Ramp, Or Not To Ramp. That Is the Question.... And Others...
« Reply #9 on: October 17, 2008, 09:33:51 AM »
You'll be doing Crinkle Cut next !! ;D ;D :'(
Not me driving the engine - I'm better looking.