Cherry plywood machining advice needed

[archis]

I have a partition project in the near future that will need to be cut from 1/2 inch cherry plywood. It will need to have a very clean cut since both sides and the cut edges will be visible.

After trying to cut out some jigs from baltic birch it has become clear I need some advice since my jigs have been pretty torn up by the bit.

What bit, feed rate and rpm would give me the best cut?

Thanks

[steve_g]

Jim

Since I don't know what your level of experience is ... I have to ask. What bit are you using? I will suggest a quality compression bit if that isn't what you're using already. Plenty of others have suggested speeds and rpm's for various bits on the forum so I will just add that my experience is that when cutting Baltic Birch the "sweet spot" seems to vary slightly from day to day batch to batch. Listen to the bit and use [shift]+[>] or [<] to make on the fly adjustments. Also, if your drop side cuts are better than your keeper side cuts... change climb vs. conventional.
Hope this gives you a starting place to find what's right for you!

Steve

[bleeth]

Jim:
All 2 sided panel products cut better with a compression bit. If my nesting is tight I will use a 1/4", for cabinet parts that get drilled in the same process I use a 5mm, and for general use I sometimes use a 3/8".
Feed and speeds will depend on your machine (PRt, PRS, Alpha, Standard, 4G, spindle, etc). I always recommend a quality solid carbide bit. Lots of info on this elsewhere in the forum as well.
BB when cut correctly will come out very clean as will cherry ply (particularly a decent domestic)

[garyb]

Jim, you already have been given sound advise above
just check if using a compression bit that you use a short upcut length since you're material is only 1/2"
Gary

[archis]

I have no experience with getting clean cuts on plywood:D

Could you recommend some compression bits? I'm not clear on exactly what they are.

Thanks

[steve_g]

Jim:
A compression bit cuts up on a portion of the bottom and down on the remainder. The net result is that all chips are "compressed" toward the center giving no tear out of the surface veneer. To realize this benefit however it is necessary for you to cut full depth in a single pass.
Asking what bits are quality bits are kind of like asking about ones' religion... seems to be very personal. I will tell you that no one will disagree that the Onsrud bits are quality ones. check Gary's web site.

Steve

[dlcw]

Jim,

Mortise Compression bits is what you need for this project.

Try some of these:

http://www.carbideprocessors.com/vortex/3100xp-xtreme-performance-compression-spirals/

They are REALLY sharp (extremely important with expensive material) and cut very clean.

With my PRSAlpha 96x60 with 2.2hp spindle, I first cut in a climb direction leaving a 1/32" skin. I then do a through-cut conventional and it leaves a super clean cut ready for edge banding. I cut 3/4" gold-ply at 4ips for first pass and 3.5ips on last pass. Spindle speed 12K rpm. This is the "sweet spot" for my machine. Baltic Birch I cut at 3.5ips on first pass and 3.5ips on second pass and get a super clean cut. Your mileage may vary. Be careful with the shift < and > changing speeds. As has been mentioned on this forum a few times, when doing this, ramp speeds are not adjusted accordingly so you could end up with cornering problems.

What I found with bits is that when cutting expensive stuff (or melamine), I ALWAYS use a new bit, not a resharpened bit. This has produced the best results. I price in bit purchases when bidding a job to make sure the customer gets the cleanest job possible.

[dlcw]

Here's another option for bits. These particular bits are for melamine and such but ToolsToday has some good bits I've used.

http://www.toolstoday.com/p-5638-cnc-compression-spiral-bits-for-mdflaminate-2-flute.aspx

[steve_g]

Let me amplify on what Don has cautioned about when using [shift]+ [<] or [>] . These "on the fly" adjustment are for tweaking speeds for the reasons given. However if major speed change is needed (I recently had a decimal point in the wrong place) short of re calculating your tool paths you can use the "on the fly" changes, Pause and resume. the ramping issues are recalculated upon resumption.

Steve

[archis]

Thanks Guys as usual lots of great advice!

I do need a couple of clarifications:

Steve,

What should I be listening for to find the "Sweet Spot".

Don,

I'm not familiar with the concept of a "climb cut". Could you or someone explain what that is?

Thanks Again.

[steve_g]

What should I be listening for to find the "Sweet Spot".


The old adage is "feed a screaming bit" something experience will tell you.

If you were hand holding a router, the direction where the router wants to grab and run away from you... that's a climbing cut. very difficult and dangerous to do with out a CNC to control the feed rate.

Steve

[archis]

Is the climbing cut an option I set in Partworks when I generate the toolpath?

[dlcw]

Jim,

I've attached a zip file that will explain it with pictures.

[bleeth]

Jim: It's time for you to look over the tutorials and videos available on the software and your machine.
After you look them over do it again more slowly and take notes on anything you didn't understand so you can go over that section again.
When hit with an expression like "compression bit" if you don't know it, google it. Lot's of info out there for a minimum of research on your part!

I'll disagree with one comment made:
"To realize this benefit however it is necessary for you to cut full depth in a single pass."
You do have to ensure that your first pass is deeper than the upcut portion of the bit. So if you have a mortise compression bit with a .19 upcut length then you need to go deeper than that on first pass. 1/4" is safe all around.

[bruce_taylor]

I have used onsrud 60-123 and 60-121 3/8 inch with good results at 11,000 rpm and 2.5 ips 3 passes. May be a little conservative but I get a nice clean cut. Just my two cents (worth about a penny these days). Good luck!

[steve_g]

Excellent document! Did you create it Don?

Steve

[archis]

Thanks everyone, I get it now. I'll get a compression bit and start experimenting.

[steve_g]

Is the climbing cut an option I set in Partworks when I generate the toolpath?




Yes, The image shows the option in PartWorks.

Steve