PDA

View Full Version : G-Wizard?



Tenson
21-10-2012, 12:45 AM
I was just wondering how many of you put faith in G-Wizard for calculating speeds and feeds?

I broke 3x 3mm bits over the last week so thought it was time to get a bit more technical about it. However, I notice that what G-Wizard suggests is different from what I have read on this forum, mostly it uses higher spindle RPM. For example I know Jonathan likes to cut aluminium using a single flute 6mm bit at 8000RPM and 600mm/min. However G-Wizard suggests more like 13000RPM. Though actually I just noticed now, it suggests pretty much what Jonathan said for an HSS cutter instead of carbide.

I broke my 3mm cutters on acrylic. I understood that it is best to have quite a high feed rate and a low RPM or else the plastic can melt. However, G-Wizard suggests that for a 3mm cutter with 3mm cut depths, I should use 22000RPM (!) and 770mm/min. IS this what you would expect, or is it going to melt the plastic? I haven't tried it yet as I need to get more 3mm bits, lol!

I also notice that it never seems to use more than about 0.2KW of cutting power which seems a little odd, do most tasks really need so little? Additionally it seems to love TiALN coated cutters but I thought that only really made a difference for really hot milling applications, not cutting plastic for example.

Jonathan
21-10-2012, 11:24 AM
I think G-Wizard is pretty good, but a bit of common sense always helps.


I broke 3x 3mm bits over the last week so thought it was time to get a bit more technical about it. However, I notice that what G-Wizard suggests is different from what I have read on this forum, mostly it uses higher spindle RPM. For example I know Jonathan likes to cut aluminium using a single flute 6mm bit at 8000RPM and 600mm/min. However G-Wizard suggests more like 13000RPM. Though actually I just noticed now, it suggests pretty much what Jonathan said for an HSS cutter instead of carbide.

Not sure where you read that - I use 600mm/min and 12600rpm (or thereabouts) for that cutter. If it's in one of my posts let me know as I should correct it.


I broke my 3mm cutters on acrylic. I understood that it is best to have quite a high feed rate and a low RPM or else the plastic can melt. However, G-Wizard suggests that for a 3mm cutter with 3mm cut depths, I should use 22000RPM (!) and 770mm/min. IS this what you would expect, or is it going to melt the plastic? I haven't tried it yet as I need to get more 3mm bits, lol!

For me it suggests the same rpm but 1300mm/min with single flute, however it also says the tool deflection will be too high if the cutter is longer than 18mm, hence the cutter is likely to break. Perhaps try a lower depth per pass and use the shortest tool you can. Bear in mind the tool deflection is proportional to the length of the tool raised to the power 4, so every little helps a lot.


I also notice that it never seems to use more than about 0.2KW of cutting power which seems a little odd, do most tasks really need so little? Additionally it seems to love TiALN coated cutters but I thought that only really made a difference for really hot milling applications, not cutting plastic for example.

Yes, but you still need your 2.2kW spindle to have enough power over the whole speed range.

Tenson
21-10-2012, 02:02 PM
Thanks for the reply Jonathan. I thought it said 8000RPM in your video showing a 6mm flute at 600mm/min but I was wrong it doesn't say about the cutter speed.

riche543
22-10-2012, 11:47 AM
I'm no expert either , snapped plenty of bits myself, I use 3mm (2 flute) to cut my 4.5mm acrylic as well. Here's the settings gwizard gives me @ 2.25mm per pass its: 20428rpm & 1052 mm per min. (this gives me a nice finished edge hardly needs cleaning up) I have read before that you should only cut at half the depth of cutter width ie: 1.5 with 3mm bit. Here's gwizards settings for 1.5 per pass : 21005rpm & 1273.8 mm per min. These settings are with gwizard set at conservative low.
Hope this helps, good luck , I know how it feels too keep breaking bits, still do while trying too cut 3mm 5005 aluminum sheet it's like bubble gum :-)
Cheers
Riche




Sent from my iPhone using Tapatalk

Tenson
22-10-2012, 04:35 PM
Thanks, I just tried some cutting again with the suggested feeds and speeds of G-Wizard and it doesn't melt the plastic as I thought it might. I guess the key is getting enough chip-load not to cause rubbing.

I'm cutting 8mm sheet, so I did multiple 3mm pass' at first with a 6mm cutter and then did a finishing pass at full depth removing 0.5mm of material. The end result is very good but there are still some very slight snipe marks. I need to sand and buff it afterwards for a real smooth finish. I tried flame polishing it with a butane pen torch but I think the flame is not hot enough as it looks a little patchy.

Jonathan
22-10-2012, 04:48 PM
I guess the key is getting enough chip-load not to cause rubbing.

When cutting plastics and aluminium that is exactly what you need to to. With other materials, such as wood, you tend to get away with too small a chipload as it just wears the cutter faster, instead of immediately breaking it.


I'm cutting 8mm sheet, so I did multiple 3mm pass' at first with a 6mm cutter and then did a finishing pass at full depth removing 0.5mm of material.

When I need a good finish on something made from aluminium I cut the part 0.1mm or 0.2mm oversize, then do a finishing pass at full depth, so long as it's not thicker than 25mm which is rare. You could try leaving less than 0.5mm as the lower force on the tool may make a difference, however the chipload may be too small unless the feedrate is increased...