Feeds speeds for v2-50

[J. C.]

Hi- I am new to this and wonder if anyone has compiled a starting estimates for v2-50 speeds and feeds.
I was using the 8500 rpm for the spiral part demo, which I think is compiled optimum for a V2-10, and kept getting pullout of the Harvey one flute that came with the pocket NC.
I know the v2 can go fast but has more pullout issues, is there some guidelines to start from? Is faster generically better for pullout issues (lower chip load at same feed rate)
Is there is limit to the sfm of things like delrin?
Any other tricks to reduce tool pullout?

Thanks
Jason

[Matt Moore]

Hi Jason,

Welcome to CNC and the Pocket NC. 

I'd suggest starting out at the tool manufacturer's website. So if you have Harvey Tools, use their search box to find that endmill's speeds and feeds. You mention the Harvey one flute endmill, here is Harvey's website on that endmill:

http://www.harveytool.com/ToolTechInfo.aspx?ToolNumber=52508

There is a speeds and feeds link in the middle of the page. LOC = length of cut. I don't mess with plastics but at 8500rpm, you may not have enough torque and may need to increase spindle speed. Additionally, you may be taking too big of a stepdown or stepover. 

Check out this video as well: https://www.youtube.com/watch?v=zzzIpC39WUg

Let us know what settings you are using.

[J. C.]

Hi Matt, thank you for the welcome. This is my first time learning CAM and CNC but I've done a modest amount of manual machining.

I am not 100% certain of the feeds and speeds used on the spiral demo, since I only have the gcode handy. Whatever was in there, it pulled the tool out badly (I know it is 8500 rpm). I got through the demo part by cutting feedrate to 50%, which worked well enough.

On my own part, also out of Delrin, I have used a couple of values below.

All if this is done with the Harvey 52508 1/8 single flute for hard plastic milling. Which unfortunately is now broken.

I had some success for a couple of hours of machining with the next parameters, but the tool eventually pulled out about 2mm on 26mm initial extension.
S 20000
F 15.8 in/min (400mm/min)
FPT. .0008"/t. ( .02mm/t)
Adaptive
Optimum load 0.75mm
Roughing stepdown 2mm
Climb cut

These parameters caused pullout in a couple of minutes:
S20000
F 20in/min
FTP .001
Adaptive
Optimum load 1mm
Roughing stepdown 4mm

I got better results at the 20k spindle speed, should I push to 35 or 40k?
Is that stepdown/ radial engagement just too high for a v2-50?
I can turn it down 2x but seems so close to the edge even if I do. It makes me nervous sitting a factor 2 away from failure, and even then the MMR goes down very low.

The 20k nearly successful numbers are leads than the Harvey table recommends. They suggest
.0056"/t for Delrin at 800-1200SFM.
.35xdia which is just over 1mm at
1x diameter. Which would be 3.1mm

For my nearly successful parameters, am nearly 8x down in FPT at less radial engagement and stepdown. I get the spindle doesn't have that much power, but still I thought I was being conservative. The spindle sounded fine.

The other thing about my system is that this is a used one I picked up recently, it wasn't that old when I bought it. It looks brand new, was barely used. But I wonder if the CHB collet is ok. If these speeds/feeds seem reasonable, I may try a new collet. I have cleaned this one meticulously.

It would also be helpful to know what others are getting away with, so that I can troubleshoot.

Thanks for any help.
Jason

[J. C.]

On a related note for the collet, does anyone know if that tiny oring that is near the back of the collet is needed, and if so, what size oring is it?
Mine is missing. Might have been me when I was checking the collet health.
Jason

[Matt Moore]

When you say, "but the tool eventually pulled out about 2mm on 26mm initial extension", what are you extending? Are you leaving the NSK spindle alone and moving the endmill so that it sticks out 26mm from the spindle? Or are you moving the spindle from the ER collet 26mm? 

Harvey recommends for that tool:

800-1200 SFM 

.0056 IPT 

.35 x Dia Radial

1 x Dia Axial

So if we aim for the middle of 1000 SFM, this is around 30,500 for spindle speed. 0.0056IPT is 430mm/min or 16.92913 inch/min (if I did my math right. I work with mm and it's the weekend). Then the stepover should be 0.04375‬inch (.125 * .35)  or 1.1mm. Stepdown of 1/8 inch or 3.175mm. So you're not far off there except for the spindle speed.    

I think you are seeing pullout because of the shape of that single flute endmill. You might have better results using 2 or more flute endmills. If the endmill is extended and taking +2mm of cut, that places a lot of torque on the spindle holder because of the way that one flute is shaped. Here's 5 options to try: 1) Try a 2 flute or more endmill. 2) Loosen the ER collet that the spindle sits in and move the spindle forward 15mm. This will let you push the endmill 15mm further into the spindle - allowing the spindle more surface area to grip on the endmill. 3) Check your collect and spindle to make sure it's working properly. Especially if you're missing parts. 4) Bump spindle speed to 30,500 5) slowing the feed rate down.

I'd try 1 through 4 and only do 5 if necessary.

And food for thought, you may want to check out Xander's CAM setup of the pocket here: https://www.youtube.com/watch?v=_s2O9-XjH_4   - just to double check you have CAM set up right (if you're not using Fusion you can download it and use it for free on an educational basis until you go commercial).

[J. C.]

Thanks for all of the leads- I have some reading to do.

I think I will try a two flute end mill- at worst it will produce half a chip load twice as often- more continuous- it's not like carbide is going to wear out quickly machining delrin- the chips- my bench near my enclosure looks like it snowed black Delrin. I searched and somehow found that tiny oring in the flurry of chips- I consider that my first miracle of the week. I did a closer look and I am not sure I am happy with the way the collet looks- I may just buy another one and try.

I have the tip of the end mill sticking 26mm from the face of the collet- producing 26 mm of tool clearance- my part is 2" in diameter and I have some removal to center. So I can't get away will a shorter stickout of the tool. I think the default for "tool #10" in PocketNc library is 1.25" for this tool, so I am shorter than the default. 

I did not move the spindle in the ER40 collet it lives in, though imagine I will one day.

I might try to use my big mill to remove some of the stock so I have less machining to do with the Pocket- just needs more setup up at the beginning to orient the part to account for the lost material. 

Has anyone had success with downflute end mills instead of upflutes? At least the push would be opposite- so if it slipped it would get shorter as opposed to over-machining.  Hard to fix once overmachined.

[Graham Stabler]

A single flute endmill is perfect and I never run lower than 30krpm except for some drilling. I've never had any pull out with reasonable parameters. I have extended my spindle out from the collet by about 17mm which covers me for most things. Just looking at one of the last parts I made in Delrin, with a 3mm single flute I ran at 40k, 1500mm/min, 3mm step down and 0.5mm optimal load. 

You should also check the collet it properly installed. With the collet UNclamped and with something in the spindle (cutter or dowel) use the supplied wrenches to snug it up, it does not need to be tight, just remove any play, the springs in the clamp assembly do the real work.

Cheers,

Graham

[Josh Pieper]

Graham,

I'm curious what you mean by "extended my spindle out from the collet by about 17mm"?  Are you using an alternate collet, or some sort of physical extension?

J.C.,

I will second Graham that the V2-50 has torque and pullout problems if you try to run below 30k.  Traditional feed and speed calculators are only of so much use for this class of machine.  You really have to run the RPM fast and take light cuts, no matter what the tool manufacturer recommends.  If you look back through Ed Kramer's IG history, you can find some workable feeds and speeds for a variety of materials and tools: https://www.instagram.com/ekramer3/

I have also found that I can get significantly more pullout resistance by using the 4mm collet and 4mm tooling.  

Josh

[Graham Stabler]

On the V2.50 the NSK spindle is itself held in an ER40 collet so I am talking about extending the spindle not the tool.

Graham

[Graham Stabler]

And to be clear by extend I mean slide out.

Graham

[J. C.]

Thanks for the suggestion to check out ekramer. 

I found a video of him machining delrin with a 4mm Datron mill at 37000 RPM, 1300mm/min feed rate, 10mm stepdown, and 0.6mm radial engagement. 

His MMR is 30x what I am doing with my 1/8 single flute Harvey when I experienced pull out.

I ordered new collets for my machine (1/8" and 4mm) from Pocket along with the 4mm Datron they offer. I will give his numbers a try, maybe a little less aggressively. (maybe 5mm stepdown and 0.5mm engagement) for roughing out my part- this would be plenty fast for now. 

I may re-try the Harvey again another day, but since I have plenty of room in my roughing operation I can use the 4mm for now.

I'll let you guys know how it goes.

Jason

[J. C.]

Thanks for everybody's help. The 4mm Datron in the 4mm collet seems to work wonders. Not being as aggressive as ekramer, but also don't want to fumble around with aggressive settings. 

I used the following- 

3d adaptive

5mm stepdown

0.5 optimal engagement-climb only

37k spindle

1200mm/min feed

26mm tool stickout (tool is 40mm OAL)

Spindle sounds like it is working but not bogging. No pulllout issues so far (4-5 hours of machining time)

This looks like a workable roughing solution for Delrin. Just documenting what I did for others if they need it.

Jason

[vect...@gmail.com]

Glad to hear you are getting good results now. That Datron 4mm single flute with 4mm shank diameter is easily my favorite endmill on the V2-50, especially in engineering plastics. It runs pretty well in aluminum too. I have rarely experienced tool pullout on the NSK spindle, even with 1/8” and 3mm shank tools and collets. One thing I do here is wipe the tool shank down with IPA sprayed on a small microfiber cloth before inserting into the spindle collet. Any debris or oil (even from your fingers) on the shank can really degrade the collet holding power. At least it seems to work well for me. 

—thanks, Ed Kramer

Instagram: @ekramer3