Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: HimyKabibble 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.
-
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
-
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.
-
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
-
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.
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.
-
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.
-
Oh another thing about ramping is you will tend to chip the material rather than getting streamers which you will with plunging.
Hood
-
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.
-
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
-
You'll be doing Crinkle Cut next !! ;D ;D :'(
-
You'll be doing Crinkle Cut next !! ;D ;D :'(
One step ahead of you Jim, already done them ;D Had the feed almost there with the 40mm U Drill but just a tad too slow.
Hood
-
In the lathe, with carbide inserts I always increase my feed to break up the chips. This works great for roughing,
but for finish cuts you don't have much choice, but the stringers aren't so course. Most of my stringy chips come from drilling
with large drills ( up to 2 inch diameter) in stainless, these could take off a hand. >:(
Ed
-
Ed, yes standard twist drills can be a real pain, on a drill press or a manual lathe you just stop feeding for a fraction then start again and that breaks the chip. Pecking does exactly the same but it can take a few goes before you get the depth of peck just right. I am starting to use U Drills now and they are the dogs dangly bits, thank goodness for eBay or I wouldnt be able to afford them.
Hood
-
Hood,
What do you mean by a "U Drill" ? ???
BTW, there is another drill peck cycle, don't know off hand what the gcode is,
but you can set a short peck with a dwel l, instead of retract, which breaks up chips, and is faster.
Works good if you don't have a real deep hole . I've used it already, and know it works.
Ed
-
Like this Ed, they are amazingly quick to drill with as you can get the spindle speeds way up and an added bonus is you can also use them to bore out as well. Not sure if you are meant to do that but I do and they work great :)
Hood
-
Hood,
OK, We call those carbide insert drills, has coolant thru. and pops out a disk when it breaks thru.
They are great, but expensive. :o
Enclosed pics of some tools I made for a production shop. The long one is a 4" or 4.5" diameter,apox 16" long insert drill with a .500" stub drill in the center.
It was used to plunge thru a steel forged yoke. Worked great. this was used in a verticle lathe,otherwise called a boring mill.
The other tools were used for boreing ,counter bore and champher all in one shot. saved on tool changes. These were used on a horizontal machinig center.
All were machined from 4140 pre hard.
Ed
-
No way I would have any U Drills if it wasnt for eBay, couldnt justify the cost as I dont do production work.
Some nice tools you have made there.
Hood