PDA

View Full Version : Make a circle out of 2" plate on a CNC?



rsr911
12-16-2005, 02:10 AM
Hey guys, I cut circles on my CNC all the time but now I've got a question. I need to make a D1-8 adapter for a 6" 4-jaw flat back chuck I bought for my big lathe so I figured I'm cut the holes for the pins and set screws as well as rough the ID and OD on my CNC. For thge center hole I figure I'd drill a big hole on the manual mill and then just loop a circular pocket cycle til I cut through the bottom of the plate. For the OD I figured I'd cut a circle say 0.060-0.100 deep and loop it but I'm afraid of breaking the endmill what if I modifiy the circle loop to cut say 0.250 over size then to size before looping down to the next depth? I plan on using a 0.500" carbide long flute endmill, do you think I'll be able to clear the chips enough to keep from breaking the endmill in such a deep slot? Should I run a bolt circle drill cycle a little bigger than the OD first or will the interupted cuts give me trouble? What if the bolt circle was oversize enough that the endmill is always cutting something and just use the holes to clear the chips? I figure I could drill holes and leave only about 1/8" web to support the disk will I do the ID. I have to do two bolt circles anyway for the pins and set screws.

Anyone have a better idea? What would you do?

All of the finish work will be done with the adapter attached to the lathe spindle, well except for facing the back of course for than I'll just chuck it in the big 3 jaw. BTW the adapter will be about 9" OD with an ID the size of the chuck.

------------------
-Christian D. Sokolowski

DR
12-16-2005, 09:47 AM
You don't say how thick the plate is, do you?

Dawai
12-16-2005, 09:49 AM
ON Adrians site, there is a easy way to cut circles with a torch, then spin it on your lathe to make it perfect.

I used a torch adapter on my cnc, a long bar to hold the torch over a barrel, you cranked the bed upa nd down to get the height right.

I almost burned the shop down. I'd suggest something different

rsr911
12-16-2005, 10:06 AM
Oops, yep thickness that's the problem, it's 2" plate! Anything less that 1/2-3/4 and I wouldn't worry about it but at 2" thick I'm concerned about chip removal. I'm running two nozzle flood coolant BTW.

------------------
-Christian D. Sokolowski

BobWarfield
12-16-2005, 10:09 AM
"Anyone have a better idea? What would you do?"

I'd buy some round stock in the correct size.

Best,

BW

debequem
12-16-2005, 10:19 AM
You could nibble away at the top until you are 1" deep and then flip the part over and repeat the process.

At least your maximum depth will be about 1", which is closer to your 3/4" don't worry zone.

Dawai
12-16-2005, 10:27 AM
Other easy fix? buy a backing plate of the correct type. Save the 2" thick for a bender. or??

Tinkerer
12-16-2005, 10:57 AM
Well you could find some one with a water jet cutter and have them rough the OD and ID with a +1/8" - 3/16" tolerance and then finish in on the mill. A simple two circle cutting op would cost about the same as the busted .5 cutter with you supplying the plate.

Mike Burdick
12-16-2005, 01:15 PM
Since it's chip removal you're worried about, couldn't you just hold the shop vacuum near it and have it suck the chips out while it's running?

Evan
12-16-2005, 01:22 PM
The guys at the local job shop cut circles like that all the time with their CNC torch rig. Probably about a 20 minute job for them and clean as heck. Just a skim cut to dress it up afterward. You might look for someone to do that for you.

mochinist
12-16-2005, 05:35 PM
Predrill a hole that will be close to the outer edge of your hole that you will be cutting, make it atleast as big as your endmill, this will be your plunge point and pause point. When you program it, write in a M00 right before it goes to plunge to the next Z depth cut, the M00 will pause the machine till you hit cycle start again and allow you too vacuum or blow out the chips with some compressed air. I also like to bolt down the center cut material that you are removing, itkeeps the piece from jumping around when it breaks loose, and prevents you from losing an expensive cutter.


Edit: also I wouldnt take more than a .250 per pass on the depth, with a .500 endmill, I might even take less than that.

[This message has been edited by mochinist (edited 12-16-2005).]

torker
12-16-2005, 06:45 PM
<font face="Verdana, Arial" size="2">Originally posted by DR:
You don't say how thick the plate is, do you?</font>
DR...yup,,,he did...the title says 2" plate.
Christian...we flame cut these sizes all the time.
I just made a set of hubs for an air boat drive. All out of 1 1/2" thick plate.
These where flame cut to within (roughly) 1/16" then machined on the lathe.
Sounds far simpler than what you are trying to do.
Mind you...this is dinasour tech that I speak!
Russ

Smoking Crater
12-16-2005, 07:39 PM
If I was you, I would lay out the I.D. and O.D. on the plate with chalk and rough out each with a hand torch. I would not worry about accuracy because you are merely removing excess material. Get as close as you dare and remember that the cut will probably be tapered one way or the other. Leave yourself enough material to account for this. I would suggest starting the cut with a 1/4" drilled hole to avoid the molten metal spray when you initially pierce. Then use lathe or mill to do the final cuts. If you can, grind the cuts to remove the hardened layer that results from the cutting. An endmill will cut through this layer, but grinding wheels are cheaper. When I cut thick plate with a hand torch, I like to wiggle the torch side-to-side to create a wide kerf so I can see what is going on. Take your time and use a face shield. A tinted face shield (#3) works well for seeing the cut, but sunglasses (like the safety glasses type) will work just as well. Take your time. After the metal changes state to a liquid, give it the cutting oxygen and pretend you are using water from a hose to wash the metal away. Good luck.

torker
12-16-2005, 08:22 PM
I always use a circle cutting jig. You can get very nice circles with these. I've had great results with up to 3" thick plate(Using an LA torch with a #6 tip...8 to 10 acet/50 O2).
As was suggested...leave some to cleanup with a grinder of your choice. Once you grind through the scale it will cut easy with end mills etc.

rsr911
12-16-2005, 11:17 PM
Sorry, no torches involved on this project, too hard on Carbide endmills. I could easily chuck this piece in my 4-jaw and cut it as well but that's not the point. For a D1-8 backing I need 6 1" holes with a setscrew hole right next to them. I want to drill those holes as well as cut the center hole and outside on the same setup on the CNC so when I mount the backing plate to the lathe I won't have much work to do to finish it up. I like mochinist's idea best for this. And M00 stop is easy and can be incorporated into a loop with ease. Heck I'm gonna have three tool stops in there anyway to spot drill and drill the different hole sizes and then to an endmill for the ID and OD. Also if this works well I'm going to want to make two more backing plates and a face plate. It's like when I made sets of soft jaws for the 3-jaw as well as the CNC's twin vises, if I need more I just load stock and walk away or do other things. Soft jaws for the vises are cut entirely in one pass and then after installation I have a program to step the tops inline with the X-axis.

I suppose I should have specified I only want to do it on the CNC and I'm looking more for ideas for the best way to accomplish that. The M00 will work nicely and with enough coolant a lot of the chips will flow out of the stop hole anyway.

------------------
-Christian D. Sokolowski

mochinist
12-17-2005, 12:00 AM
Glad I could help, and I hope it works out nicely for you, it has worked well for me in the past.

snowman
12-17-2005, 12:49 AM
yup, drill a starter hole and just interpolate. long carbide endmills chatter a bit, but if you hit them hard with flood coolant and go light on the feed, you'll be ok.

can't you use a larger diameter endmill?

I would actually think that a good HSS rougher would be better in this situation. It'll handle the vibrations better.

-Jacob

rsr911
12-17-2005, 03:23 AM
Maybe I'll try the rougher. Yeah I could go with a larger endmill, I've got holders all the way up to 1". Let's say I use a 3/4" HSS rougher, what kind of DOC would you take? I normally like to use a high feed and speed and take real light cuts. One job I run at 32 IPM, using a 1/4" endmill and only 0.025" DOC. I find I get the smoothest circles this way especially if I program in decel overide G99. Only time I ever have trouble with that method is if I'm cutting hot roll as the mill scale eats the tools much faster.

------------------
-Christian D. Sokolowski

mochinist
12-17-2005, 11:23 AM
With roughing mills I usually use the diameter of the tool for my depth of cut. Personally I like the higher feeds and lower depth of cuts, it is easier on your machine and alot of times it is way faster.

rsr911
12-17-2005, 02:24 PM
<font face="Verdana, Arial" size="2">Originally posted by mochinist:
With roughing mills I usually use the diameter of the tool for my depth of cut. Personally I like the higher feeds and lower depth of cuts, it is easier on your machine and alot of times it is way faster. </font>


I've found that to be true for me as well. It was suggested to me by a pro 5 axis operator/programmer. I cut these little disk blanks about 1.5 dia. out of 1/4" plate. He recommended 80IPM and 0.010-0.020" DOC with a 1/4" endmill going about 4000-5000 RPM with lots of coolant. I can only get up to 32 IPM so I run those disks at 0.025" DOC, 3500 RPM and 32 IPM. They come out great for the second op.

I stopped by the tool supply house this morning and picked up a 63/64" bit, a spot drill, a 1" reamer, and a 3/4" roughing endmill will 2.5" flutes. I figure since the machine can run all day with me only watching I'll run conservative on both the feed, speed and DOC. I'm figuring 0.250" DOC, 250 RPM, and 2.5-3 IPM. If it works well I'll make my other adapter and a face plate.

spope14
12-17-2005, 02:40 PM
Use a G02 cycle, not a circular cycle (sounds like you are using a canned cycle to do this.

First off, cut the plate down using a bandsaw to about 6 1/2 inches across for a 6 inch finish piece. also, cut the corners off as best as you can. In this way, you have little chip issue, and less propensity to cutter binding. The plate will look like an awkward stop sign.

For programming. Lead the cicrlc in to create cutter compensation, then program around the part, then lead off, return, then go again.

Here is an example, 6 inch circle, program zero is centerline of part:

G01X-4.5, y-1.5 (could be closer)
G01 z-.060 f3.0
g01g41 d1 x-3.0
g01 y0
g02 x-3 y0 R3.0 (hopefully, the machine will do a complete circle)
g01 y1.5
g40 x4.5
g0z.100
x-4.5 y-1.5
g01z-.060

on and on. You could sub program the circle part for repeat use, or if you need IJK center coordinates, this would be I3.0 j0

If you need to program in circle quadrants this is the routine...

G01X-4.5, y-1.5 (could be closer)
G01 z-.060 f3.0
g01g41 d1 x-3.0
g01 y0
g02 x0y3 r3.0
g02 x3.0 y0 r3.0
g02 x0 y-3 r3.0
g02 x-3 y0 r3.0
g01 y1.5
g40 x-4.5
g0z.100

I would use cutter comp, and most likely a 3/4 end mill to rough, set at .020 oversize of diameter in the comp, this leaves .010 to .020 finish stock on the part. Then do a finish pass with a 1/2 end mill set to actual size, or the same 3/4 cutter with the diameter set at actual - use a different diameter offset number (call out d2 instead of d1 in a comp line). Do the finish pass two depths, say z-1.00, and z-2.050. This prevents cutter flex.

No cutter comp? using a 3/4 end mill, here are your points for the circle alone, starting points remain the same

G01X-4.5, y-1.5 (could be closer)
G01 z-.060 f3.0
g01 x-3.375
g01 y0
g02 x0 y3.375 r3.375
g02 x3.375 y0 r3.375
g02 x0 y-3.375 r3.375
g02 x-3.375 y0 r3.375
g01 y1.5
g01 x-4.5


Just my 2 cents.




[This message has been edited by spope14 (edited 12-17-2005).]

rsr911
12-17-2005, 04:10 PM
spope14,

What if I want to clamp it in my vise on the outside of the rectangle?

My machine cuts circles in quadrants and needs I and J for each line, I do it all the time like that just on much thinner metal. As far as the finished size of the OD I'll true that up once the adapter is mounted to the lathe, same with the ID as well as a boss for the small 4-jaw.

You've got me thinking though. I suppose a good way would be to CNC drill a center hole and the bolt and pin circles like originally planned. Then remove the part and cut like you say on my band saw. I could then recenter it on the table and use two of the bolt holes to clamp it down and then cut the OD and ID. I'm just going to loop a quadrant circle with a G91 Z movement in there.

------------------
-Christian D. Sokolowski

spope14
12-18-2005, 03:44 PM
If I were doing this, I would do the inner circles and all drilled holes and bosses first in one operation. This sets all dimensions to the inner circle for reference. Mill in the center hole if you can. I would clamp this on the ID with a strap clamp across the face, or bolt the plate down using any through holes you might drill in on Op 1. The ID hole, being milled, would make an excellant place to indicate a center off of for the outside surface to be milled. I would not want to "jump clamps" when milling an OD, nor continually re-clamp on the OD to make the part as things do shift.

IJK's are easy to determine using quadrants.

You can loop the cycle, or sub program it. Either way works, programming is something there are 100 ways to do the same thing with, and all 100 ways are correct.

Good luck, I would be interested in receiving how you did this, and your code.

What is your control you are using?