Radius Dish Carve is estimated at 13 hours

Hey everyone,

I am trying to carve a Radiusing Dish for building acoustic guitars with CNC, and used a 1/4" ball nose finish toolpath for my design. It's a 24" diameter circle, with a 350" subtle arch carved into the material (MDF) throughout the circle. I designed it in Fusion 360, and my makerspace uses VCarve, so I'm trying to create the toolpath there.

With a 10% stepover, it's telling me the carve time is 13 hours. Is there a way to reduce this? I tried one toolpath with a Raster strategy, and another with a Climb strategy, and both were over 13 hours.

Any help would be appreciated.

Hi CM - What is your feed speed? You will have to max this out to reduce time.... 10% step over is 0.6mm (very fine) you could use 1.0mm and take some time out. I usually use a 1/2" coving for that sort of thing. A bigger stepover just means a little bit more sanding. So 1.2mm stepover will take 13/2hrs plus 30mins sanding... A spiral strategy will reduce time as there are no stop/starts if it has that. Are you roughing then finishing or straight to finish? Do some test cuts of 1.0mm 2mm and 3mm stepover to establish what sanding time would look like. Use a 1/2" coving tool so the radius is big ie the scallop is small. Fusion has spiral strategy so look at that....Peter

https://www.facebook.com/ScootCNC/vi...3884215086398/

As Pete says, doing a roughing pass and a finishing pass will save time, rather than trying to do it all as a finishing pass. Try waterline roughing with the biggest tool you can fit and a 1/3 tool diameter stepover, then following up with a circular strategy. You don't have to use a small diameter tool unless you've got detail you need to get into; a large diameter ball nose is better for something like the interior of a bowl, since the cusps (or scallops) are shallower. Raster means that the tool is going back and forth in parallel passes; climb refers to the direction it's going in. You can do both at the same time, but a circular strategy (spiralling in or out) would be more efficient for a circular bowl shape. Climb vs. conventional doesn't make much difference in MDF.

Thank you both for your thoughts. For some reason, the "Makerspace Edition" VCarve I'm using doesn't allow me to select a 3/8" or 1/2" ball nose. Just a 1/4". I'm sure when I'm at the space their system will allow it though, I just can't test it at home.

When you say a "Spiral Strategy", I'm guessing you mean for it to carve in a circular pattern? I tried 2 different paths -- one with a Circular Pattern, and another with a Raster Pattern (where it went back and forth up the entire shape), and both were about the same amount of time.

If I do a roughing first, does that mean I can use a larger stepover with my finishing path after it's roughed out? If so, what stepover or speed would you recommend after it's roughed?

Thank you both again for your thoughts and tips!!

Hi Stewart - As fast as the machine will go. Generally you can create your own tool in that sort of software. Every tool will not be in the library. Yes spiral is a circular cut - it will start at the edge or in the middle up to you.
Roughing and finishing depend on tools and your speeds available. You need to figure what is the max speed of the machine as this will give you the least path time.

What router are you using and what size spindle is it? This will define your potential depth of cut (DOC). If you can cut the deepest part of the radius in one cut then you can cut the part in one go. If you can on;y cut say 50% of the deepest part then you will have to cut in two goes.... You need to do some test cuts to figure this out plus you need to tell us what tools you have available. Use the biggest meanest sharpest tools you have... Peter

Thanks Peter! It looks like I'll have to do some investigation & testing to nail down how I'm gonna do this. I really appreciate those thoughts. Huge help, and gives me hope that I can get this thing done.

- Colby

Hi Colby - a 24" dish (610mm) with a 350" rad (8890mm) has a depth of 5.3mm in the middle. This is 0.21" or just over 3/16". This is easily machined with a one flute 6mm tool or I'd use a 10mm round end tool. So I expect if your stuck with a 1/4: round tool, then you can cut it in one with some hand finishing or rough it to 0.5mm then do a fine finish cut,. But this depends on your cutting time. I assume you want to do it in one "opening" time of your Makerspace. So find out what max speed your machine can feed at. My last machine ran at 10-15m/min for this sort of thing. My current machine runs at 3-4m/min... Peter

So I'd rough in one direction and finish in the other direction then a quick sand. If spiral is there and its fast that would be the go. But cutting in only X or Y maybe faster then spiral if your machine does not do two axis simultaneous machining fast... A machine may do the gantry direction faster and the z up down vs the direction that uses two motors plus the Z... Look at the specs or do some test air cuts in X and Y and figure the machines max speed vs direction. Peter