Are Perfect Circles Achievable? Any tips on cutting Polypropylene

[zeke]

Does anyone have experience with cutting perfect small circles? I'm not having much luck, the quality is not impressive at all. I must be doing something wrong. I'm including some pictures that show the results. I have a 2009 PRSstandard 48x96 w/a 4HP spindle.

I used a profile cut with a 1/2" 48-072 Onsrud bit with a 16k spindle speed, a feed rate of 102 ipm and plunge rate of 18.

Another problem I encountered with the poly is melting. I was trying to drill some 1/4" holes through 1/2" sheet of poly, the holes were not very good quality mostly due to the melting. Unfortunately I don't have a Bot-drill only a spindle for this. Also the poly tends to attach to the bit and it gets very bad after maybe 4-5 holes drilled, then the poly on the bit starts to score the material.

Do you think I will have the same issues with melting on type1 PVC?


4947


4948


4949


4950


4951

[team08]

I never thought bits would make that much of a difference until I called Onsrud for application help. I cut a lot of plastic, and their O-Flute bits are AMAZING for plastics. They cut like butter. Go buy some immediately and enter my world of amazement! Slow spindle speed and medium speed make plastic effortless. I don't even want to cut wood anymore. Okay, enough ranting. But yes, go get yourself some O-Flutes...

[Brady Watson]

Zeke,
You are most likely cutting too fast (guessing you are cutting something like a .875" diameter pocket for the quarters?)

1st try adjusting your VR settings - specifically your XY Move Ramp Speed. Change this to .2 - this sets the slowest speed that your tool will move. Then pull down your 102 ipm speed (102 IPM = 1.7 IPS) to .2 to .4 IPS (12 to 24 IPM) and see how the quality looks. If you get melting during cutting, you might want to switch to an Onsrud 63-series tool. If the bottom of the pocket's finish suffers, they have an O-flute that is made specifically for a clean bottom finish. Straight fluted tools generate too much heat in some plastics, causing gummy edges and rewelding of chips.

In regards to drilling plastics, the best results are acheived using an inside profile strategy (circle vectors) using a smaller tool than the hole itself. A .125 or .1875" tool would be fine. In some cases, cutting the holes undersized (say .22" in diameter) and then coming back with a .25" tool to drill precisely should give you the best of both worlds.

-B

[Gary Campbell]

Zeke...
The geometry of that bit will not yield good results as it is designed for composites and wood. The attack angle of the carbide face chips the surface, rather than shears it off. I also think that you should use a smaller diameter bit to allow the tool to move faster.

Both Acrylic and PVC solid are difficult but possible to cut with a little experimentation. I would use an Onsrud or Belin 3/16" single O flute at somewhere around 45ipm and 8-12K rpm. 1/8" diameter if the material is less than 1/4" thick. These bits do not SOUND good when cutting well so watch the cut edge for your desired results while you increase/descrease the move speed/RPM. It seems each brand of material has its own sweet spot, sorry I can be more specific.

You may want to cut these with a .010-.015 final pass allowance for the best results. I sometimes remove the slug between passes to make sure there are no extra pieces of plastic to heat up when cutting the final pass. An air blower helps remove chips and cool the bit to help eliminate remelting of the chips.

EDIT: Or what Brady says!
Gary

[zeke]

Are these same bits recommended for any plastic including type1 PVC? Thanks gents, I'll work on your recommendations.

[Gary Campbell]

Zeke...
I use them for both. The PVC seems more dense than acrylic, but like the acrylic it likes to melt. I cut the piece shown below from type 1 gray with a 1/4" O flute, including the reinforcement rings using speeds similar the above.

Brady makes a good point about the VR settings. I set mine according to his article a while back and forgot to mention what a difference that it makes.

4952
Gary

[zeke]

Thanks Gary! An intriguing piece of work!

[zeke]

I talked to Onsrud. Gary, was that a 1/4" Onsrud 63-700 (hard plastics) or 63-750 (soft plastics) series O flute that Brady was referring to?

[Brady Watson]

Onsrud 63-700 Series - Hard plastic and solid surface plastics

Provides a smooth finish in hard plastics with upward chip removal. Helix angle=21°

Usage: Acrylic, nylon, PVC, polycarbonate, and solid surface
_________

Onsrud 63-750 Series - Soft plastic, hard plastic, and solid surface.

Gives a smooth finish in soft plastics with upward chip removal. Helix angle=30°

Usage: HDPE, HIPS, UHMW, ABS, polycarbonate, PE, polystryrene, polypropylene, acetal, acrylic, PET, and solid surface
_________

Either of these tools will work fine for what you are cutting, with the -750 Series being a little more versatile. It appears that the -750 Series seems to do everything the -700 one does, but this starts to enter into the nitty-gritty of fine tuning after you have dialed your tool in for a given material. Note that the important thing here is the O-flute geometry. It is designed to cut away quickly, with the helix shoulder of the tool falling away quickly, to reduce friction, heat and melting. The helix angle is not as important, although this depends on the material. Bear in mind that whichever one you chose, it will be a night & day difference compared to what you are using now. They last a very, very long time if you only cut plastic with it.

-B

[zeke]

Excellent, thanks Brady, I'll be ordering tonight. I was also thinking about purchasing some drill bits from Onsrud after talking with them. They said at a low speed these drill bits can be used to produce good quality drill size holes without melting the plastics. I would need to run my HSD 4HP spindle at 1-2k RPM's according to Onsrud. I'm still new at this, the spindle always start at 6k RPM's, so I figure I need to do some research to see if this will be an issue or if it is even capable of going below that range and without damaging the equipment.

I would use the 63 series for routing, profiling, pocketing, etc. Do you feel the drill bit is a good quality option?

I'm also going to purchase some 90degree bits, they recommended the 37-50 series.

[Brady Watson]

Your spindle may stall below 3000 RPM, depending on your plunge rate. I would try ordering ONE drill to see if it will do the trick, with the option of using a regular end mill or drill going forward. If you do profile cuts (cut the inside of each hole with a spiral plunge via PartWorks, undersized) - then come back in to shave off/ream the .03" remaining material with an end mill, drill etc, I don't think you will have much problem with welding.

-B

[zeke]

Good deal Brady, thanks for the information. I placed my order, should be a fun-filled weekend!

[zeke]

I got to thinking a little bit more about Gary's note about the air blower. Is there a link to an example of a good configuration?

[Gary Campbell]

Zeke...
This one works...$20 @ McMaster...

4953
Gary

[zeke]

Gary, found it, thanks. Are you using a compressor or air pump for the air source? I have a fish tank pump I was thinking might work as the source with some clear tubing running through the echain to the hose.

Zeke

[Gary Campbell]

Zeke...
It comes of my compressor @ 90psi. I do have a flow control on the tube to adjust the flow. I dont think an aquarium pump will work... but you can try and report back
Gary

[gerryv]

Zeke, You mentioned two issues; quality of cut and out-of-round circles. Please let us know if the good advise on bit's speeds, etc. solved the second problem as well. Thanks much.

[zeke]

The advice absolutely improved the quality of the cut, thanks for the helping hand! The O-flute bits made a big difference as well as the speeds. I found to produce the optimal results of the cut on polypropelene I used a profile cut with a spiral plunge recommended by Brady using a .5 IPS on the feed rate and 8K on the RPM's. This configuration produced a good chip, eliminated the melting and it looks like about 98-99% of the disfigured circle cut. There is still a barely noticeable straight (vs. circular) imperfection on the circle cut that is in parallel with the X axis in the same place on either side, however I realized a major improvement. I haven't tried the air blast yet to add to the bit cooling, I ordered the flex hose and will add that accessory soon.

I think I need to go back and do a professional job of squaring in concert with surfacing. I initially squared the machine when I first put it together and had been holding off on the surfacing until today.

Does anyone have a best practices / techniques for surfacing and squaring. I made a surfacing file, that was fairly straight forward. When I began to surface my hardwood plywood, I noticed a section wasn't being touched and I was shaving about 1/16" off the top. The surfacing was also producing lines, I'm attaching a picture. I wanted to surface the base board first to get a good start on quality from the ground up.

I stopped the surfacing and checked the rails with both a carpenter's level and square. I put a light on the back side of these measuring tools and there was light everywhere between the rails and both the level or the square. I'm hoping these aren't quality measuring tools for the CNC, otherwise, I may have allot of shimming to do. I'm hoping it is the 48x96 plywood that is imperfect which seems the most likely root cause. I wouldn't think I would have a depression on the rails for only about 6-8 inches. Also other areas on the rails where I viewed light did not have the same surfacing issue adjacent to that area. The challenge is trying to figure out if I even have an issue.

In regards to the lines from the surfacing, it appears my Z may need a slight adjustment. I have the single rail gantry and took a look around, doesn't look like there is much room for adjustments. Any hints? Has anyone fine tuned their machine enough to receive no lines? This is good information to have for planning cuts. I guess I'm concerned that any pocketing scenario may always yield lines.

I found this Tram gage, would you recommend it for squaring?
http://perfectible.info/us/manufacturing-and-metalworking/bridgeport
http://www.youtube.com/watch?v=s7yHkZP3flQ



4954

[rb99]

I would be interested in knowing if the 1% that is not a perfect circle is your machine, all Shopbots, or a problem with the SB software and how it handles arcs and lines etc...

Maybe there is a way to get a number of different owners to do a standard test to see if everyone has this problem?

RIB

[zeke]

Interesting thought. Looks like the first link I provided in my previous post has dynamic content and is no longer useful. Too late to edit the post, the second/youtube link should work. I'm including another link that I hope is more static for the Tram gauge. This product has a fairly good price tag versus some of the others I've seen. Would you guys recommend this gauge?

http://cgi.ebay.com/Tram-Gage-to-Square-the-Spindle-of-Bridgeport-mill-head_W0QQitemZ250470085528QQcmdZViewItemQQptZLH_De faultDomain_0?hash=item3a512e3398&_trksid=p3286.c0 .m14&_trkparms=65%3A12%7C66%3A2%7C39%3A1%7C72%3A12 05%7C293%3A1%7C294%3A50#ht_2865wt_1122

[beacon14]

I made a trammel gauge out of a piece of wood, a drill bit, and a pencil. Take a strip of scrap wood maybe 1" x 1" x 20" long. Drill a hole in one end just large enough to snugly stick a pencil into. Wrap some masking tape around the pencil if needed for a snug fit. Drill a hole in the other end with a 1/2" drill bit. Now jam the drill end of the bit into the hole, and chuck the shank of the 1/2" bit into the router. The pencil should be at the other end of the stick, pointing down towards the table.

Of course the router is never turned on during this entire process. By making a larger diameter trammel you do not need micrometer accuracy. If you can adjust your Z axis to get the pencil tip to vary from the surface no more than 1/16" over a 36" diameter circle, that will equate to less than .002" with a 1" diameter router bit.

The pencil and drill bit are still usable, so the only cost is the strip of scrap wood.

You can make a decent surfacing file by drawing a rectangle a little larger than your table in PartWorks, and using a Pocketing toolpath with Raster selected instead of Offset. With a back and forth cutting action you may still see stripes even with almost perfect smoothness due to the opposing cut directions of the alternating stripes.

[2talltary]

Found some good info on PVC at http://www.iplasticsupply.com/materials/pvc-poly-vinyl-chloride-sheet-rod. They have data sheets and whole bunch of stuff that might help.

[bleeth]

A botter in Canada (Paco) wrote a surfacing program for hardwoods and surfacing your table that works well. Here's a link to it:

http://pacosarea.blogspot.com/2007/02/surfacing-along-axis-shopbot-routine.html