hardwood profile cutout advice -- my first paying commission!

[bking1836]

Hi everyone,

I have my first paying commission and am looking to mine the wisdom of the forum.

I've designed a funky modern curvy bench that will have custom metal legs that someone else is making.

I cut a short prototype out of scrap 3/4" plywood with pretty good results. But I basically know what I am doing with plywood and a good compression bit, and the client wants it out of 3/4" thick ash. I have pocketed and v-carved ash before with very good results, but I'm worried about all the profile cutouts.

Here's the bench slat:
31170

And a representation of the little spacers:
31171

They come together to look like this:
31169

For test cuts of the slats and spacers out of ash, I used a 1/4" upcut, .2125" depth 12000 rpm and 3ips, all of which more or less fits with what the SB calculator suggests. The first slat did fine(ish), although that bit really wanted to lift the stock off the table. Indeed, the first spacer got ripped loose and sucked away into the DC system (definitely learned that 1 tab won't do). On the second slat the bit started slipping in the collet and I aborted. I might not have tightened the collet enough, but in any case that leads to my big question:

How would you approach cutting this job in terms of bit selection, feed rate, pass depth and rpm? Also, edge quality really matters, especially on the top, so climb cut with a .01" allowance and then do a full depth last pass (stick with climb or conventional?)??

I have an essentially brand new PRS Standard with the 2.2 spindle. I have 1/4" upcut, downcut and compression bits and a 3/8" upcut bit at my disposal.

I appreciate any advice. I really want to get this cut right the first time!

Thanks,
Brian

[Joe Porter]

There is a brand new tutorial on the Vectric Portal website about using compression bits and toolpathing them. I am sure you have an account. Personally, I think 3ips @12000 rpm is a little too fast and too low. I would try 2ips @16000 and see if I am still making chips instead of dust. If your bit is slipping in the collet and it is tight, the collet may be packed with saw dust. Take it apart and blow it out each time you change bits. Hope this is of some help...joe

[chiloquinruss]

EVERY time I think I have ALL the answers, I learn something new! ;) Some of the wood I've been cutting lately is like my arteries, it's really hard ;) and sure is different that the last time I cut it!

Anyhow, I have shifted to using just a little faster spindle speeds and making a couple more passes that normal. I have also added just a tad to my tabs (a little longer and a little thicker, more tabs is good).

On those little pieces you might want to not cut all the way through (leave an onion skin) and sand the excess off after the cut. I have a supply of small parts in my DC as well! ;)

Have fun and good luck on your first for-pay gig! Russ

[Tim Lucas]

I second Russ on both, make more passes and leave a skin on to be sanded off.

I cut some small parts out of Bass wood (soft) with a compression bit. I bring my material down to just over a half inch, cut depth is half inch, then to the drum sander we go. Sand the back side till they come loose and clean the parts up. I never have them come loose. Hard wood I would use the upcut to keep things cool and clear but would cut shallow cuts so I would not pull the part up.

Tim

[robtown]

I second Russ on both, make more passes and leave a skin on to be sanded off.

I cut some small parts out of Bass wood (soft) with a compression bit. I bring my material down to just over a half inch, cut depth is half inch, then to the drum sander we go. Sand the back side till they come loose and clean the parts up. I never have them come loose. Hard wood I would use the upcut to keep things cool and clear but would cut shallow cuts so I would not pull the part up.

Tim
I would use a larger diameter cutter. Looks like you could use up to a 1/2” bit there.

[knight_toolworks]

I pretty much cut wood at 3ips 1/4" pass 10k rpms. then a cleanup pass. tabs on wood are a little with the grain are safest but they are the most fragile. on the end grain they are stronger but you risk tearing the grain. so I make them thicker and bandsaw the parts out of the wood.

[bking1836]

Thank you to those who responded. I appreciate the advice. I have had some luck in the past with faster, shallower passes with a downcut, which is probably the direction I will go...I guess!

What amazes me is that there doesn't seem to be any sort of default for through cutting hardwood. If you're cutting 3/4" plywood, for example, a simple default is to use a 1/4" compression bit with 1/4" passes. But there doesn't seem to be such a default with hardwood, especially a harder species like ash. I realize people's machines and spindles/routers can vary drastically, but for the beefier machines with spindles like a ShopBot, I feel like there should be some guidance that's relatively reliable to follow.

I am having a blast with the CNC...I just had no idea there were so many gray areas!

[Brady Watson]

But there doesn't seem to be such a default with hardwood, especially a harder species like ash. I realize people's machines and spindles/routers can vary drastically, but for the beefier machines with spindles like a ShopBot, I feel like there should be some guidance that's relatively reliable to follow.

Every piece of natural material is different. The grain of the wood, the density and structure varies from board to board. There is no hard rule for cutting natural materials. Only through careful observation and listening to the tool can you dial it in to where it needs to be. Somewhere in the middle is best. Start by picking the feed rate and RPM that gives the best finish and then work on harmonics by adjusting the RPM. Chipload calculators are for maximizing tool life, NOT cut quality.

Nobody mentioned hold down & how important it is to cut quality. If the part vibrates because it isn't held down firmly, edge quality goes out the window. Also, keep in mind you are routing & not milling...the spindles sold by SB only reach their full horsepower rating above 12,000 RPM. Lower than this and you pull more amps and put more heat into the motor windings. (This also wastes electricity because the motor isn't operating in it's most efficient range. ) Crank that sucker up & route!

-B

[bking1836]

Every piece of natural material is different. The grain of the wood, the density and structure varies from board to board. There is no hard rule for cutting natural materials.



Thanks Brady. I agree. I'm not looking for a hard rule, just a that starting point -- the "somewhere in the middle" from which I can fine tune. Some people say take 1/4" passes with a 1/4 upcut at 10k rpm and 2 ips for ash; others say 1/8" passes at 16000 rpm at 3 ips with a downcut. Etc. I know there's more than one way to skin a cat, but these are pretty different approaches to achieve the same result!

Enough people have cut out oak or ash parts on a ShopBot enough times that there should be some sort of best practice starting point out there. As a relative newbie, that's my wish I guess!

[knight_toolworks]

oak is like baby wood try purple heart or ipe or suck (G) yes wood likes to vibrate it needs a stronger hold down. here are some tap handles I make out of walnut. I nail between everyone with plastic nails to keep vibes down and cut speed as fast as practical. there is also my air powered clamp for making hollow boxes in a strip. the hose holds the boxes much better and kills all the vibrations I got with the toggle clamps.

[Burkhardt]

Maybe I missed it but is this job a one-off, small series or larger series production? Your speed/feed/bit size optimization strategy may depend, also how you hold it down. For small quantity the tabs may be O.K. and the feed etc. is not that critical because you will spend anyway more time preparing and finishing. But for larger quantity of all the little blocks I would probably drill/mill the holes first and make a custom fixture with suitable dowels to hold the parts for the cutout (downcut bit) without tabs.

As for the final product, you may have to somehow chamfer the sharp edges or they could leave unwanted patterns or splinters on users' posterior.

[bobmoore]

Those small parts in hardwood can be a pain even with good vacuum hold down. If I were doing this job I would run these as fast as possible and leave a large tab (1 inch wide .25 tall) on one of the straight sides. Make sure the vectors were straight lines of coarse , then run the parts through a table saw to remove the tabs. For safety have the parts on the off side of the blade so you don't pinch them with the fence.

[bking1836]

Maybe I missed it but is this job a one-off, small series or larger series production? Your speed/feed/bit size optimization strategy may depend, also how you hold it down. For small quantity the tabs may be O.K. and the feed etc. is not that critical because you will spend anyway more time preparing and finishing. But for larger quantity of all the little blocks I would probably drill/mill the holes first and make a custom fixture with suitable dowels to hold the parts for the cutout (downcut bit) without tabs.

As for the final product, you may have to somehow chamfer the sharp edges or they could leave unwanted patterns or splinters on users' posterior.

At this point it's a job that I will run only a few times. I never thought about a jig or fixture for this. Very interesting idea. As for people's posteriors, I plan to ease the top edges of the slats with sanding sponges. It will also get a spray lacquer finish, which will help.

Ultimately I'd like to iterate the design to eliminate all the small spacers -- which I think is possible with two long slotted slats that run perpendicular to the main slats in place of the spacers. But I have to figure out how to transfer the geometry and create some sort of notches so that everything lines up.

[bking1836]

Those small parts in hardwood can be a pain even with good vacuum hold down. If I were doing this job I would run these as fast as possible and leave a large tab (1 inch wide .25 tall) on one of the straight sides. Make sure the vectors were straight lines of coarse , then run the parts through a table saw to remove the tabs. For safety have the parts on the off side of the blade so you don't pinch them with the fence.

Great idea about the tabs and TS. A 1" wide .25" high tab in ash should hold pretty well. I like using the bandsaw to get through tabs, but I'm working with larger stock than usual for this job. Thanks.

[knight_toolworks]

or taller and shorter like 1/8" long and .5 tall or more thats easier to sand. that pic I posted has those tabs .

[jTr]

Great thread - cool jigs - I love the air hose clamp idea!

I just completed a project that involved flip-ops for 64" long, arc'd 8/4 hard maple strips. 2" wide with 1/4" groove down the center on both flat faces. First time in 6 years running the machine that I had to do flip ops. Used clamps on ends of the rough stock and set dowel pins in table for flip alignment.
What I learned:
Forget the tabs. Leave an onion skin .125 thick - ( think "full tab"). Radically improved cut quality - just need to go to bandsaw for a quick release of parts from rough stock. High quality flush trim bit to clean up.
1/4" bits are to be abandoned with this density and thickness of lumber. Chips jamb/burn /packing = slipping and broken bits. 3/8" is essential for harder woods. Use a chip breaker bit if you can.
Up-cut is probably best. Still had a few jambs with a compression, leading to packing/burning of chips on a few pieces.

Good luck!
Jeff

Wish I'd heard Brady's comment sooner about the RPM's to power. I've been fooling myself thinking I'm babying the machine keeping things at 12k or lower. Works for plys, but will try higher RPM's on future projects.

[bking1836]

What I learned:
Forget the tabs. Leave an onion skin .125 thick - ( think "full tab"). Radically improved cut quality - just need to go to bandsaw for a quick release of parts from rough stock. High quality flush trim bit to clean up.
1/4" bits are to be abandoned with this density and thickness of lumber. Chips jamb/burn /packing = slipping and broken bits. 3/8" is essential for harder woods. Use a chip breaker bit if you can.
Up-cut is probably best. Still had a few jambs with a compression, leading to packing/burning of chips on a few pieces.

Good luck!
Jeff


Thanks Jeff! I can foresee projects where that approach would be really helpful. This time, I am pretty much stuck because I started today. Got the ash all lined up in VCarve and on the spoilboard and drilled all the 3/8" and 1/4" holes, as well as 33 hold down screws! I ran out of time so I left the computer and shopbot on, and tomorrow morning I will do the through cuts. I am holding my breath.

31188

After I read your post I went back into Vcarve to see if I have room for the 3/8" upcut to do the through cuts. It's possible for the bench slats, although it's tight and I worry about the integrity of my tabs/hold down. A 3/8" bit is a no go for the spacers. Is it worth trying just for the slats?

If not, my strategy will be to use a 1/4" downcut at .16" deep passes, starting at 2.5 ips and 12k rpm. I will adjust feed and rpm on the fly based on sound. For better or worse, I've broken enough bits that I can identify the warning sounds.

[bking1836]

or taller and shorter like 1/8" long and .5 tall or more thats easier to sand. that pic I posted has those tabs .

I think this is part of the answer for me today. Thanks!

[bking1836]

Update for anyone who might be interested....I cut one of the ash panels this morning -- the one with 64 spacers and 2 slats. I used the 1/4" downcut at .162" passes. Ran at 2.5 ips and adjusted rpm to 12500 up from 12000 during the cut. It screamed a bit, as 1/4" bits do, but it cut without incident. Edge quality is decent.

31189

The narrow, tall tabs (.25" x .65") worked quite well. No issues with parts rattling or coming loose. I placed them on the back and bottom of the pieces where any residual after sanding essentially won't be seen anyway.

So now I have the remaining 30 slats to cut. I didn't love how it sounded when the first two slats were cut on the first panel...I wonder if I need to slow the feed rate down. The spacers were fine at 2.5 ips, but they are so small that I doubt the machine ever actually went 2.5 ips. I'd switch to the 3/8 upcut but I just don't have enough room for adequate and proper holddown.

[scottp55]

For kicks and giggles,
If using a climb cut with the downcut...swap to a conventional profile pass.
Most of my downcut bits prefer it on profile passes.
Feed is in the ballpark, tweak rpm's and then increase both proportionally until quality suffers...then I usually back off 10%.
Like everyone has been saying...Listen to it:)
2 cents.
scott

[bking1836]

For kicks and giggles,
If using a climb cut with the downcut...swap to a conventional profile pass.
Most of my downcut bits prefer it on profile passes.
Feed is in the ballpark, tweak rpm's and then increase both proportionally until quality suffers...then I usually back off 10%.
Like everyone has been saying...Listen to it:)
2 cents.
scott

So I tried switching to conventional, and wouldn't you know it, but the conventional cut edge quality is better than climb cutting! Not by a lot, but still better. Thanks! In this most recent run, I ended up pushing feed rate to 3 ips and, although I tinkered with rpm, I keep coming back to 12500. As I go higher than 12500 the pitch of the whine starts to get really high. As it is this 1/4" bit is pretty unbearable to listen to!

I didn't appreciate this at first, but having 32 slats to cut out is giving me quite the opportunity to tinker with settings...

[dlcw]

Last year I made chairs for my dining table out of solid bubinga. Bubinga is INCREDIBLY hard, dense wood. Legs were cut from 1.75" thick boards. I used a 3/8" 2-flute downcut spiral. Feed was 4IPS, spindle was at 13K RPM, with a 2.2HP spindle. Pass cut depth was set at .25" Went off without a hitch. All the legs and curved arm rests were cut perfectly.

As each machine is different, feeds and speeds will vary. I ALWAYS ramp when cutting, solid wood, plywood or other material. Don't get carried away with high spindle speeds. I tune speeds and feeds according to cutting sound. If the bit is screaming, it's hungry. You either need to speed up your feed rate or slow down your spindle speed. If the spindle appears to be lugging a little, speed up the spindle or slow down the speed. Eventually you will discover where YOUR machines sweet spot is for different types of material. Record this in a journal of some sort or create your own file of feeds and speeds. Manufacturer recommended settings are just that, recommended. It is just a starting point for you to determine your "right" settings.

When cutting any hard materials, I always climb cut leaving about 1/32" skin. I then conventional cut that last pass. I've noted flex in my machine, even though I tune it after every large cutting job. The climb cut pushes the bit away from the line. The conventional cut pulls the bit to the line. And since you are cutting very little material on that final pass, machine flex is minimal. Yes it takes longer but the results are predictable and of very high quality. Just part of the learning curve.

[Brady Watson]

Bubinga IS hard, Don. I forgot how hard it was until last weekend when I made a little something for the Mrs. I found myself going back and recutting the edges with .007" allowance full pass to clean up the stepdown marks.

-B

[dlcw]

Brady, I've found that with the flex in my machine, I don't have to leave an allowance when doing the climb/conventional cut process. There is enough slop that the conventional cut has material left over to cut after the climb cut is done. This is especially true with all the plywood I cut. I climb cut 3/4" ply with a 1/4" compression bit in two passes. That seems to be enough side force on the bit to push it away from my cut line a tiny fraction. Then the conventional cut cleans the cut up right to the line. The more force you apply to the bit in the climb cut, the further the bit will be pushed from your cut line.

Bubinga makes oak look like pine in regards to hardness. It is some tough stuff. However, because it is so dense it is also brittle. I've bought LARGE pieces over the years that had micro cracks in it from when the tree fell over. Kinda interesting.

Attached picture is of the chairs I made. The table can be seen also. The table is solid resinous (gummy) cherry with bubinga bread board ends. The base is solid bubinga.

http://www.talkshopbot.com/forum/attachment.php?attachmentid=31193&stc=1

[scottp55]

"I've bought LARGE pieces over the years that had micro cracks in it from when the tree fell over. Kinda interesting."

Interesting Don. JUST surfaced some Red Gum a Desktopper brought me in his suitcase from OZ almost 2 years ago. ZERO visible checking until I cut off the paint squaring the ends with a Freud thin kerf crosscut finish blade, and then surfaced it for 2 parallel sides. And 4 surface splits showed up in 24 hours, and one end is horrible checking now(even though coated Linseed/beeswax within 20 minutes and it was acclimated to shop)!

Funny, even the Desktop will leave watermarks from .25" bit flex from woods B.Walnut up, but even making a last pass depth of .02" will clean it up a bit from Sugar Maple up in hardness. Spiral ramp profile pass will fool the eye until you try to sand the end grain to 400G.
Offsetting a full depth pass like Brady says with a spiral ramp, personally leaves the least sanding for me from Sugar Maple up to Teak/Bloodwood for me.
2 cents to the Masters:)
scott

[Brady Watson]

Beautiful stuff, Don. You're right - it really does make the common woods look like pallet material :)

I bet those chairs will last for 100 years+. They've got to be so dent/gouge resistant that they'd be too nice to get rid of...and I totally get the wheels! Sucker must weigh every bit of 40 lbs!

-B

[dlcw]

Beautiful stuff, Don. You're right - it really does make the common woods look like pallet material :)

I bet those chairs will last for 100 years+. They've got to be so dent/gouge resistant that they'd be too nice to get rid of...and I totally get the wheels! Sucker must weigh every bit of 40 lbs!

-B

Actually Brady the chairs weight in about 25lbs. Not to bad really considering the wood. For finish I used about 4 coats of MLCampbell Duravar. Tough stuff. One of my daughters has already put dibs on it when I kick the bucket. I think it's fair since she helped me build the table and all the chairs.

[bking1836]

Last year I made chairs for my dining table out of solid bubinga. Bubinga is INCREDIBLY hard, dense wood. Legs were cut from 1.75" thick boards. I used a 3/8" 2-flute downcut spiral. Feed was 4IPS, spindle was at 13K RPM, with a 2.2HP spindle. Pass cut depth was set at .25" Went off without a hitch. All the legs and curved arm rests were cut perfectly.

As each machine is different, feeds and speeds will vary. I ALWAYS ramp when cutting, solid wood, plywood or other material. Don't get carried away with high spindle speeds. I tune speeds and feeds according to cutting sound. If the bit is screaming, it's hungry. You either need to speed up your feed rate or slow down your spindle speed. If the spindle appears to be lugging a little, speed up the spindle or slow down the speed. Eventually you will discover where YOUR machines sweet spot is for different types of material. Record this in a journal of some sort or create your own file of feeds and speeds. Manufacturer recommended settings are just that, recommended. It is just a starting point for you to determine your "right" settings.

When cutting any hard materials, I always climb cut leaving about 1/32" skin. I then conventional cut that last pass. I've noted flex in my machine, even though I tune it after every large cutting job. The climb cut pushes the bit away from the line. The conventional cut pulls the bit to the line. And since you are cutting very little material on that final pass, machine flex is minimal. Yes it takes longer but the results are predictable and of very high quality. Just part of the learning curve.

Thank you Don. Very helpful. I should probably add a 3/8 downcut spiral with 1.25" or 1.5" CEL to my ever-growing inventory of bits.

So I'm happy to report that all 94 pieces have been cut successfully. In the end there was definitely more drama in my head than on the spoil board. The conventional cut left a better edge for sure, and I ended up being fine at 3ips and 12500 rpm with .162" passes and a 1/4" downcut bit. I wonder if I could have pushed the cut depth a little deeper...

All that ash turned into this pile of parts:

31194

And here's the rough assembly:

31195

I'm pleased with the design and how it all came together, but it was definitely more work than I had anticipated. And I'm not even done yet!

For this design to be commercially viable, I will need to find some efficiencies. Interestingly, the problem wasn't prepping the stock (my lumber mill will take rough sawn 4/4 stock to 3/4" S3S for pennies), nor is it the machining, which set up pretty easily and will run relatively efficiently next time. It's the 94 parts to thread onto rods, plus sanding and finishing, that takes so much time and effort!

I appreciate the wisdom and support of this forum.

Brian

[knight_toolworks]

Bubinga IS hard, Don. I forgot how hard it was until last weekend when I made a little something for the Mrs. I found myself going back and recutting the edges with .007" allowance full pass to clean up the stepdown marks.

-B
yep and purple heart and ipe. thats what I cut my teeth on and man wasted some wood. i tested on pdf then tried purple heart and learned the machine had slop (G)