# What is the most effective way to carve a bowl/tray?



## Greengecko (Aug 13, 2020)

I'm pretty now to the CNC world, just got a machine three months ago. I've tried different ways make bowls and trays:

1) Using a two-flute bowl bit, which doesn't work well when working with maple cause it's too hard and I don't get a smooth cut
2) Using a large ball nose to scoop out and finish the whole thing, but that takes forever and dulls my bits pretty quickly
3) Using an end mill to scoop out the dish and smooth the bottom, and then a large ball nose to do the walls, for a rounder bottom edge, but then I often end up with a line or uneven edge near the edges where end mill stopped

Each method has its problems and I'd like to hear from others what the most efficient way is in order to reduce the amount of sanding as much as possible. I'm using 1" lumber most of the time, but sometimes I use 2". Thanks for any suggestions.


----------



## difalkner (Jan 3, 2012)

What machine do you have? In using the bowl bit are you trying to take off more than your machine can handle (i.e. is it flexing)? Have you tried cutting both ways - conventional and climb? Are you getting straight lines from the bit or chatter marks? Straight lines could indicate your router/spindle isn't properly trammed, chatter could be trying to cut too fast or flex in the machine or a dull bit.

Got any photos you can show us?

David


----------



## TimPa (Jan 4, 2011)

funny thing, when we make one offs with the CNC, you try to figure what will give you the best outcome and you live with what we get. sometime spending a LOT of time sanding. but when we make repeat items, we get the opportunity to "fine tune" our cnc process parameters to improve the cut quality.

i have been doing that for several months now with a repeat order (50/month). i was sanding a lot at the beginning - no fun. things to try - bits- obviously get quality carbide bits (for CNC) when you can, follow the mfr speed and feeds as much as possible, upcuts vs downcuts, lube you machine (stict-sion causes bumps), try a clean-up pass by removing most of the material, except maybe .015 - .020", then cutting that by itself (maybe use a new bit for that). try climb vs conventional on that last pass as David mentioned. these are the things i've found, in general, that have an impact on cut quality.


----------



## Greengecko (Aug 13, 2020)

I've attached a pic of a tray in cherry I just cut yesterday that's having these issues.

I've got a ShopSabre 23, and I use 1/4" and 1/2" bits. So I was using a Niagara Cutter 1/2" TiCN ball nose to do all the work (like in my example #2), which was great while it was sharp, but that got dull after a few days of doing that, so I'm trying to figure out a good long-term strategy. That bit has been leaving burn marks where the tip cuts, since that part of course gets dull first. Now I bought a an Amana ZRN 1/2" ball nose that cost me over $100 and I want to make that one last as long as possible.

I'm being very careful not to push the speeds, so I'm running the roughing passes at 30-40 in/min and the finishing at 10-20 in/min. I have the router set at 16,000 RPM. Sometimes for maple I use 19,000. The machine is well lubed, which I do every couple of weeks, and it's moving very smoothly on the tracks. We're a mom-n-pop home shop, so we don't 24-hour production or anything like that.

I was using some 3D models for bowls, but I found the quality of the walls to be real problematic, full of uneven areas. So I switched over to just using vectors and I just set the numbers for the roughing and finishing toolpaths manually, figuring out how close I can get to remove the most material before the finishing pass. But it gets tricky when trying to switch from an end mill to a ball nose - I frequently end up with a line or uneven area around the edges, between the two toolpaths. Even a 0.001" difference in height is visible in the wood.

I recently learned about the Separate Last Pass Allowance, which is great for smoothing the inside walls of the bowl, as well as the outer cut, to remove the all the marks from the multiple passes. So I have been using that and it's been a great help.

I found a flat end mill with rounded edges (cove nose) from Vortex Tool which would seem to be the way to eliminate the sharp line around the perimeter that I get from using a standard end mill. Maybe combining that with the large ball nose would give a pretty clean transition.

One thing I'm not familiar with is the Climb vs. Conventional direction -- when do you use which?


----------



## difalkner (Jan 3, 2012)

Greengecko said:


> One thing I'm not familiar with is the Climb vs. Conventional direction -- when do you use which?


In wood I have found that roughing with climb and finishing with conventional gives the best surfaces. In metal it's the other way around.

David


----------



## kp91 (Sep 10, 2004)

I use an end Mill to hog out the bulk, and finish with a bowl and tray bit


----------



## Greengecko (Aug 13, 2020)

Thanks, and how do deal with the sharp line left by the end mill?


----------



## kp91 (Sep 10, 2004)

Two separate pocket toolpaths. The endmill carves out the waste area. The bowl and tray bit toolpath cleans up after the end mill.


----------



## TimPa (Jan 4, 2011)

Greengecko said:


> I'm being very careful not to push the speeds, so I'm running the roughing passes at 30-40 in/min and the finishing at 10-20 in/min. I have the router set at 16,000 RPM. Sometimes for maple I use 19,000.


I think this may be why your bits are dulling quickly. look into feeds and speeds, there are online calculators. i had to learn the same lesson...try raising your feed rate to maybe 80-90 ipm and slow down your spindle to maybe 10k rpm. immdiately after the cut, AND the bit has stopped rotating, you should be able to touch the bit and it is cool to the touch.

im guessing the lines are from inaccurate tool length settings.


----------



## Greengecko (Aug 13, 2020)

TimPa, those feed rates sound really fast for working with maple. When I've tried faster rates, even with the RPMs at 16,000 the tool gets really loud. In the picture, the line is from the end mill clearing the bottom of the tray, and I'm not quite sure how to calculate and position the 1/2" ball nose to meet that line and remove it.


----------



## BalloonEngineer (Mar 27, 2009)

Your Shopsabre is definitely capable of faster speeds, and that will greatly improve bit life and cut quality. Burning is always a sign that feed rates are too slow for the spindle rpms.


----------



## Greengecko (Aug 13, 2020)

BalloonEngineer said:


> Your Shopsabre is definitely capable of faster speeds, and that will greatly improve bit life and cut quality. Burning is always a sign that feed rates are too slow for the spindle rpms.


I'm new to this, so I didn't know that. I thought that you had to have more speed to get through tough materials like hard maple, so I was putting it up to 19,000 RPM at 20 IPM. If I'm using a 3-flute 1/2"-diameter straight upcut spiral bit to make the inner walls of my trays, what do you recommend for RPMs and speed?


----------



## difalkner (Jan 3, 2012)

18k rpm is what I run for 99% of my jobs in all materials, from 1/64" bit up to1.5" flat bottom bit for surfacing the spoilboard - works great for me. Feed rates for the bit you mention should probably be in the 125 ipm to 200 ipm. It'll never reach those speeds on something that small, though, but at least 100 ipm.

David


----------



## ger21 (Feb 10, 2019)

> If I'm using a 3-flute 1/2"-diameter straight upcut spiral bit to make the inner walls of my trays, what do you recommend for RPMs and speed?


13,000-14,000 and 250-300ipm at 1/2" depth of cut. Even faster if your machine can handle it

I've cut plywood and particle board with a similar bit at 1200ipm and 16000 rpm, on a much bigger machine.


----------



## BalloonEngineer (Mar 27, 2009)

Greengecko said:


> If I'm using a 3-flute 1/2"-diameter straight upcut spiral bit to make the inner walls of my trays, what do you recommend for RPMs and speed?


First of all, in wood, normally use 2 flute max. The formula for Feed is:
Feed = rpm x no. of flutes x chip load 
So lets say at 16K, with a 2 flute bit, and a chipload in the .010 range, 320 ipm (480 with the 3 flute!) 
If you do not have a chipload from the bit manufacturer, .010 is fairly safe with a 1/2" bit, .005 with a 1/4".


----------



## Greengecko (Aug 13, 2020)

Those numbers seem mind-boggling to me, I'm scared to try them! I feel like the bit will be so overloaded at that IPM rate. I work mainly with cherry, maple and oak. Sometimes with padauk and purpleheart. I thought I was supposed to greatly slow down the IPM when in came to these harder woods.


----------



## ger21 (Feb 10, 2019)

The lower you go, the more heat that is generated, which dulls the bit faster. The duller the bit, the more heat that is generated, which dulls the bit faster. Vicious cycle.
Only slow down to get a better finish. Otherwise, always go as fast as possible.
Cherry and Padauk are pretty soft woods, actually.
And compared to carbide, maple is pretty soft as well.


----------



## difalkner (Jan 3, 2012)

ger21 said:


> And compared to carbide, maple is pretty soft as well.


Now that's funny! True, but still funny.  

David


----------



## Greengecko (Aug 13, 2020)

Ah, that's the issue for me -- I small in small woodcrafts where a fine finish is most important thing. So the main problem I've been having is burning the edges and corners when cutting bowls and trays, things like that. It's a killer to try and sand that stuff off, especially in the recessed areas where it's difficult to reach. I think my mistake was using a high RPM with slow IPM.

So, given that goal, what are the bits and speeds/feeds you'd use to carve a bowl in maple?


----------



## kp91 (Sep 10, 2004)

My machine is not capable of very fast feed speeds, I still get good results. Leave yourself room for a finish pass if you are getting burning. 

I've made bowls and trays with a handheld router as well, definitely not going that fast for the whole time 😉. 

Experiment and adjust as needed.


----------



## TimPa (Jan 4, 2011)

i also make many smaller projects from hardwood. i typically do not exceed 100 ipm. but i was dulling bits like crazy at 16k rpm. so if you dont want to go fast, you have to slow down the spindle to maybe 10k. this will minimize you burn, and extend your bit life.


----------



## Greengecko (Aug 13, 2020)

That's kind of the direction I ended up going because the high speeds we causing burns, and if it moves too fast, even though the machine can handle it, I don't get a smooth surface. With the large 1/2" ball nose I found that using it to make the finishing pass in a maple tray bottom, at 50 IPM and 10K RPM gave me real smooth edges. The bottom cut is very shallow, about .03", but the sides are removing 0.135" (a little more than half the width of the ball nose) which is as close as I can get when roughing with the straight end mill bit without leaving a mark around the edges. I ended up just using the ball nose to finish the entire bottom surface, because I find it difficult to exatly match the depth of the previous cut exactly when finishing, so I get a line, as pictured previously.


----------



## Greengecko (Aug 13, 2020)

What's the typical depth of cut for these faster speeds we've been talking about here?


----------



## TimPa (Jan 4, 2011)

i've seen tooling manufacturers guidelines set at 1/2 the tool diameter. 1/2" end mill set to cut at .25" depth...

these are starting points, you will likely be doing things different later on, as the need arises, but these are good hogging out guidelines.


----------

