Author Topic: seeking advice on milling 3/4 in plywood  (Read 956 times)

Offline hogman

  • Jr. Member
  • **
  • Posts: 6
seeking advice on milling 3/4 in plywood
« on: October 30, 2020, 08:02:44 AM »
Hi fellas,
I am new to cnc. I run a woodshop that makes a chair. I sell chairs at art shows. Each chair has 70 pieces of 3/4 ply stack laminated. I did this by hand and to sculpt curves I started with a 5 hp grinder using 16 grit and moved up to the finish.
My objective is to cut out 90 % of prefinish grinding and sanding out. I have cut very nice parts to date.

I made my machine. I just upgraded Z for more rigidity. Table is 48 by 48. spindle is 3.5 hp.

My issue is RPM of spindle. Calculators tell me that for ply using a 2 flute end mill speed is 3000 for 100 in per minute feed.

My machine chokes on this. I run 17500 and cuts are good without burn. But this bothers me due to discrepancy. I use fusion 360 cam and adaptive clearing does not give me option to cut in small steps down.

I use 5/16 and 1/2 inch ball end mill. I dont need speed of feed. I can go slower if advised to. Please tell me how to do this if you will.
thank you, JR


Offline philf

  • Hero Member
  • *****
  • Posts: 971
  • Country: gb
Re: seeking advice on milling 3/4 in plywood
« Reply #1 on: October 30, 2020, 05:09:13 PM »
Hi Hogman,

For metal cutting I use FSWizard ( https://zero-divide.net/?page=fswizard )to calculate feeds & speeds. I have no experience in cutting wood on a CNC.

Selecting wood (no plywood option in the free version) with a 5/16" ball ended cutter (carbide) and 0.5" depth of cut it suggests 10,039 rpm and a feed rate of 178 in/min. (1.71 HP). With 0.25 DOC it recommends 8,816 rpm with 163.2 in/min (1.28 HP)

For a 1/2" cutter and 0.5" DOC the spindle speed reduces to 5,596 rpm and the feed recommended is 109 in/min. (Spindle power 2.61 HP).

These figures are for taking full width cuts.

What's the maximum speed of your spindle? If there aren't pulleys to give you different speed rates if you're running a 20,000 rpm spindle at 5,000 rpm you may find your spindle is only capable of less than 1HP.

Phil.



Phil Fern
Location: Marple, Cheshire

Offline Spurry

  • Sr. Member
  • ****
  • Posts: 333
  • Country: england
  • Norfolk, UK
Re: seeking advice on milling 3/4 in plywood
« Reply #2 on: October 30, 2020, 05:32:07 PM »
Generally, when machining wood, the governing factor is holding the stuff. Without knowing how you are holding your material to the bed it's difficult to advise. Usually I just depend on the vacuum pump, so with a carbide 2 flute 6mm cutter I would not cut more than 3mm deep per pass. Revs would be circa 22,000 - 24000, and max speed 4m/min. The machine could cut deeper per pass, but that would mean taking extra time/effort to secure it to the bed first, so I take the easy way out.

If your software cannot step-down per pass, a possible solution could be to duplicate the contours with each consecutive contour to an increased depth. For a good edge at 18mm, I would step down in 3mm intervals for 17mm but with increased offset (0.2mm - 0.5mm.) Final cut would be to 18mm deep at the correct offset. I never use tabs either, as they seem to be detected in the final passes.

Offline hogman

  • Jr. Member
  • **
  • Posts: 6
Re: seeking advice on milling 3/4 in plywood/many thanks fellas
« Reply #3 on: November 01, 2020, 07:37:58 AM »
Thanks for the info fellas.

My spindle is 220 3.5 HP 24000rpm. My table is 1500 mm by 1500mm and I do have issues securing a 48 inch board. I clamp edges, keeping operations into a 47 by 47 box. I have tried a vac pump. I build a small box with hose to pump. this box holds well if I just put it on wool yet when I try to get it thru 3/4 in mdf waste to ply does not hold.

I have learned alot in past 9 months. One is the build of CNC. This one runs on wheels. And I see the inherent deflection. I have put Z on rails and it is much better. Yet it is reliant on X which is still on wheels.

I cut 9/64 holes an inch apart on mdf. I am thinking of one larger hole in middle of MDF to secure center of ply. That would be hugely helpful.

JR

Offline hogman

  • Jr. Member
  • **
  • Posts: 6
Re: seeking advice on milling 3/4 in plywood/
« Reply #4 on: November 01, 2020, 07:42:30 AM »
Hi Spurry, can you please explain what offset is and how to use it? JR

Offline Spurry

  • Sr. Member
  • ****
  • Posts: 333
  • Country: england
  • Norfolk, UK
Re: seeking advice on milling 3/4 in plywood/
« Reply #5 on: November 01, 2020, 01:59:51 PM »
Hi Spurry, can you please explain what offset is and how to use it? JR

I'll give it a go. What would be considered 'normal' tool offset is half of the diameter of the cutter. So if you have your outline required, the cutting path will be half the cutter diameter, outside of that outline so that you finish with your desired size.

You mentioned that you could not use your software to step-down. So just duplicate your outline. The first copy of it would be for example, using 3mm steps, cut down to 16mm deep, the second down to 13mm, and so on. The sneaky bit is that you add-on say 0.5mm onto to tool offsets so it's 3.50mm, until you get down to 1mm of thickness left. For that last cut, of 1mm deep, you set the tool offset to 3.00mm. Effectively you are taking a 0.5mm x 1.0mm cut to complete your work, which should give you a decent finish as so little material is being removed.

In practice, it's a lot easier to demonstrate than explain in words.

Offline WeldingRod

  • Sr. Member
  • ****
  • Posts: 374
Re: seeking advice on milling 3/4 in plywood
« Reply #6 on: November 01, 2020, 03:01:12 PM »
I think you want a two or three stage blower for hold down, rather than a vacuum pump.  Think "high pressure shop vac".  Unless your hardware is really well sealed,  a vacuum pump has too low of a flow rate.

Sent from my SM-G892A using Tapatalk


Offline vtsteam

  • Global Moderator
  • Hero Member
  • *****
  • Posts: 5827
  • Country: us
  • Republic of Vermont
    • www. sredmond.com
Re: seeking advice on milling 3/4 in plywood
« Reply #7 on: November 01, 2020, 05:40:13 PM »
There are all kinds of plywood so I would think the best bit speed is going to depend on the type. Douglas Fir vs Red Oak vs Occume vs Kahya for example have quite varied characteristics and hardnesses. I imagine that your experience is a better teacher than a set "plywood recommendation". I'm surprised you can't change the spindle speed via software, but also is it possible to do that manually? If you don't change plywood types during a run, seems like one setting ought to do it.
I love it when a Plan B comes together!
Steve
www.sredmond.com

Offline hogman

  • Jr. Member
  • **
  • Posts: 6
Re: seeking advice on milling 3/4 in plywood
« Reply #8 on: November 02, 2020, 11:21:44 AM »
thanks again all. super valuable information for me.

I  use fusion 360 and for say adaptive 3d, the tool will go deep at first than cut to radial setting. I have just finished running ops with the recommendation above. Just duplicated and changed the depths.

IN fusion Ramp is a 3d op that you can set stepdowns. and the 2d contour too. Yet scallop, parallel 3d adaptive do not have step down, they have the size that mill cuts radially. I have found that my ops over tax the spindle if left at initial settings.

I am now stepping down as suggested. Thank you. JR