Software for making panels on CNC

[Savvy]

Edit: I'll post my findings right here at the top to save others from reading through.

 

Software:

The general consensus on CNC software is to use the Free Personal version of Fusion 360 for design, and Estlcam for the path generation. Fusion 360 has a high learning curve but is very powerful. If you focus on '2d Sketches' it will be easier to follow. Cut2d,vCarve are very good bits of software but are quite expensive. Adobe Illustrator, Corel Draw and Google Sketchup(free) are other options.

 

After some testing and swearing, I posted my settings here:

 

 

Original post:

 

So my 30x20 CNC machine has arrived and I've got a couple of test panels, with paths all created and ready to go with Cut2d. However I see that the Cut2d Trial version doesn't allow me to export the paths so there's no way to actually see if it will work.

 

I find Cut2d to be *really* good software and was intending to buy it however I don't really want to pay the $250NZD without actually seeing how the end product will look.

 

So now I'm back to square-one a bit and looking at what software setup might be best for me. It looks like Inkscape with plugins may be able to create the Panels and Tool paths, however Inkscape is (being free) requires a lot more faffing abouth. I see Fusion360 is another option, but that has a pretty high monthly fee.

 

What does everyone else here use for CNC milling software? Should I just go ahead and buy Cut2d or is there some other software that will work better?

Edited April 17, 2021 by Savvy

[Muts]

Fusion 360 is free for Hobbyist. I use Fusion for drawing the panels and for the CNC milling I use Estlcam.

[Brewnix]

I have been using only Fusion 360 for all my 3d printed and CNC projects. Some what of a steep learning curve for me. But a bit of time and some YouTube tutorials and Googling and I manage. I had no CAD experience at all. But as stated by Muts it's free. Download the trial use it for a month and then ask for a free hobby use license at the end of the free trial. It draws in 2d and 3d objects you can save DXF and STL files. Then you are able to switch to the Manufacturing tab set tools and compute tool path's for your project for 3 axis CNC. I have not run in to anything that required me to want to pay for a sub. Other then the simulations tab. But that's another story.

[Savvy]

Thanks all, yes after some research I found that Fusion 360 was free for hobbyist.

 

I'm still on the fence on what to do. Fusion 360 looks to be more capable, especially if I want to move into creating 3d type parts in the future however the learning curve is indeed quite high. I couldn't believe how easy Cut2d was to use, I don't even recall looking at many tutorials - everything just seemed in logical places. As a software developer myself I found it really interesting.

 

Edit: After finding the "sketch" mode in Fusion 360, it suddenly makes a lot more sense for building 2d stuff.

 

I did manage to send a demo rectangle to the CNC machine to see how it would cut plastic. It was a total mess, the plastic would just melt on the bit then it would break. I found there's two different types of Acrylic, extruded and Cast. Cast being much better for milling panels.

 

What settings are you guys using for cutting the panels?

 

I started with 1mm bits but they broke, then moved to a 2mm bit but I broke this also by setting the z-depth then pressing "down" instead of "up", breaking the bit into the plastic. So frustrating.

 

At the moment I'm looking at cutting 3m cast Acrylic with these settings (I'm still testing):

• 2mm bit
• 10,000 RPM (not even sure my Chinese 2030 can do this)
• 650 mm/min travel speed
• 230 plunge speed.
• 0.5mm depth of cut per pass, so it takes 6 passes to cut through the full 3mm.

Does that sound close to what you guys are using?

 

I also secure the sheet onto the bed with double sided tape, but found the tape would catch all the shavings on the final pass, causing some issues. I wonder if this is also 'grabbing' the bit causing it to break sometimes.

 

I'm using bits that (I think) are more for carving wood - which could be causing the breakages. As I understand it a single flute end mill is what I'm after.

Edited April 12, 2021 by Savvy

[CorporalCarrot]

You're settings seem to be about right to me, but be careful with the travel speed.  As you experienced, if you try going too fast then you'll overload the bit and break it, but there is a more subtle problem you may not notice.  The 3020 machines are pretty robust, but tend to have plastic mounts for the spindles.  The plastic mount isn't very stiff, so if you up the travel speed, then there is a risk that the mount will bend slightly under load (should return to it's original shape, unless you do something seriously heavy handed with it!).  If the mount bends, then your cutter will move around.  Depending on your requirements, this could lead to parts not fitting together well (or holes being under/over size).  When I was using a 3020 chinese machine, I tended to keep speeds around the 400mm/min mark, but cutting with a slow feed rate can also increase friction (and lead to melting, as you experienced with the softer extruded acrylic. It's a delicate balance, especially for the cheaper machines!

 

With all plastics, there is also some variability in material properties of the raw sheet between vendors, and even between batches from the same vendor.  This could affect what machine settings you should use.  Ultimately, make some test passes on a scrap piece first, to help determine what travel speed and cut depth you should use.

 

As you note, a single fluted cutter is important for acrylic.  The large single flute helps clear away the chips/swarf.  If it blocks then you'll start melting the plastic again.  The waste material should come off in chips, not a continuous spiral.  If you get a big spiral, it means the cutting edge is generating a lot of friction and you'll overheat again.

 

General rule of thumb with acrylic is to set your spindle speed as fast as possible!  I use 20,000rpm on my machine for my 2mm single flute cutters.  Typicall, actual cutting speeds are measured in m/sec at the cutting tip, which can then be converted to RPM for the specific bit; https://www.cutter-shop.com/information/speed-and-feeds-calculator.html. The spindle speed and feed are linked, so if you change one, you will need to change the other.

 

Stepcraft have a pretty good guide for acrylic their machine.  You settings will differ, but the principle remains; https://www.stepcraft.us/blog/stepcraft-blog-6/post/cutting-acrylic-8-guidelines-to-get-the-best-results-1

 

The last two things to consider is whether to use conventional or climb milling and whether to use an up or down cutting tool.  I could explain conventional/climb milling, but this pdf does a better job out of the box! https://mhubchicago.com/media/240440/business/6284/Tech_ConventionalMillingVsClimbMilling.pdf  as you are using a cheap 3020 chinese machine, i'd stick to conventional machining.  You'll probably get lots of chatter if you try climb milling.

 

Up and down cutters differ by the direction of the cutting spiral.  Up cutters tend to clear swarf and chips better (as the spiral goes up), but also tends to pull the material off the machine bed (especially with bendy materials like plastic) and could affect accuracy / finish.  If you secure the plastic to your spoil board with lots of holes and screws, this probably won't be an issue.  Down cutters avoid this issue by pushing the material down into the bed, but the opposite spiral can affect clearing the swarf / chips.  I'd suggest you go with up-cutters for acrylic.

 

There is a lot to learn to get machining plastics just right.  It's a bit of a black art, so don't worry if you don't get it right first time.  Adjust your settings and try again!  Making test passes is a really good idea if you get material from a new supplier.  In my experience, suppliers materials don't tend to change much over time, but I guess if they change their production process or raw materials, then you might caught out!

 

Stick with fusion360.  Once you have figured it out, it is by far the most appropriate software for a hobbyist.  Check out their youtube channel (https://www.youtube.com/channel/UCiMwMz3RMbW5mbx0iDcRQ2g) there are loads of really great tutorials on their to help you learn.

 

Good luck!

[Savvy]

Thanks very much CorporalCarrot, that really is a huge help. Once I get everything working to a reasonable level I might post a new thread called "Settings for CNC panels" which has all the info I've found. I'm sure it would be a helpful resource for others including myself.

I'm waiting on some replacement bits so I can continue my testing. The only single-flute one I can find locally is 4mm but hopefully it's ok for cutting the outlines.

Edited April 12, 2021 by Savvy

[No1sonuk]

Regarding heating of plastic while cutting:
Try a "bit fan".  You won't be disappointed.
 

https://www.bantamtools.com/blog/introducing-the-bit-fan-a-new-othermill-accessory-you-can-make

 

A bit fan sits on your cutter's shank and blows air down as it spins, cooling the bit and any plastic chips that come off, meaning they can't melt and clog.

The down-side is that it tends to throw the chips everywhere!