Hi all,
Looking for advice on what settings I should use to pocket out this design.
I'm using a 20 degree (10 degrees each side of vertical) engraving bit with a flat diameter of 0.2mm and a 40% stepover.
Have done it once (6.5 hours!) and the flat areas seem to have a poor finish - especially in the really tight areas.
Have attached my current settings to see if I am there or there-abouts with my settings. Any advice appreciated...
willower
What settings for engraving bits?
- Adrian
- Vectric Archimage
- Posts: 14680
- Joined: Thu Nov 23, 2006 2:19 pm
- Model of CNC Machine: ShopBot PRS Alpha 96x48
- Location: Surrey, UK
Re: What settings for engraving bits?
The best way to do the flat areas is to specify a clearance tool in the pocket toolpath with a better geometry for flat areas. If you want to do it with just the engraving bit then you need to change the stepover to a far lower value (5 to 8%) so there isn't so much ridging on the flat area. It will take far longer to cut that way though so specifying an additional tool is the best way.
-
- Vectric Wizard
- Posts: 724
- Joined: Sun Jun 16, 2013 4:40 am
- Model of CNC Machine: Home Built 4-axis Router
- Location: Fort Collins, CO
Re: What settings for engraving bits?
Yes, but the feed rate is really slow at 250mm/min. I guess on most machines you could easily crank it up and compensate for the finer steps.
Dovetail and Finger Joint, Puzzle, Maze and Guilloche freeware at fabrikisto.com/tailmaker-software
- Adrian
- Vectric Archimage
- Posts: 14680
- Joined: Thu Nov 23, 2006 2:19 pm
- Model of CNC Machine: ShopBot PRS Alpha 96x48
- Location: Surrey, UK
Re: What settings for engraving bits?
I don't know if the OP is running his machine at the optimum speed or not but a finer stepover will always be slower than a coarser one which was my point.
-
- Vectric Apprentice
- Posts: 82
- Joined: Tue Jan 24, 2012 11:50 pm
- Model of CNC Machine: Legacy Maverick II 3x5; Aspire 11.5
- Location: Western Oregon
Re: What settings for engraving bits?
I have carved this calendar several times, but carved the negative of what you are showing. I have used both 45 and 60 degree V-bits. On a 16" diameter cutting it takes about 3 hours. See pic (with 60 degree V-bit)
-brian
-brian
- adze_cnc
- Vectric Wizard
- Posts: 4379
- Joined: Sat Jul 27, 2013 10:08 pm
- Model of CNC Machine: AXYZ 4008
- Location: Vancouver, BC, Canada
Re: What settings for engraving bits?
Something that has not been asked is: what material are you cutting?
If some one said to me they were getting a poor surface quality out of beech I’d be concerned but if it was lumberyard “spruce pine fir hemlock” I’d figure that’s par for the course.
The step-over is already just the thickness of a sheet of paper. As has been mentioned how about using a flat clearance tool to a) speed up the cut and b) allow a flat tool to create a flat surface?
If some one said to me they were getting a poor surface quality out of beech I’d be concerned but if it was lumberyard “spruce pine fir hemlock” I’d figure that’s par for the course.
The step-over is already just the thickness of a sheet of paper. As has been mentioned how about using a flat clearance tool to a) speed up the cut and b) allow a flat tool to create a flat surface?
- Rcnewcomb
- Vectric Archimage
- Posts: 5927
- Joined: Fri Nov 04, 2005 5:54 am
- Model of CNC Machine: 24x36 GCnC/WinCNC with ATC
- Location: San Jose, California, USA
- Contact:
Re: What settings for engraving bits?
I noticed both the Stepover and the Clearance Pass Stepover were set to 40%.
Using 40% for the Clearance Pass Stepover is fine. The help documentation explains:
Clearance Pass Stepover
Only used when a V-Bit tool is being used to rough machine at multiple Z levels down to a specified flat depth. This stepover can be much larger than the Final Pass Stepover because the tool is only rough machining material away. Increasing the Clearance Pass Stepover will reduce the machining time, but you must be careful to ensure it is not too great for the material being cut.
[Final Pass] Stepover
The distance the cutter moves over when finish machining and is usually set to be a relatively small distance to produce a smooth surface finish on the job.
Therefore, if you want the flat areas to be smoother using the engraving tool you should set the [Final Pass] Stepover to be less than half of the flat diameter. Obviously this will increase machine time. This is where you have to decide if you want to save time by using an additional tool for clearing the flat areas, or if you are willing to wait longer to avoid a tool change.
Using 40% for the Clearance Pass Stepover is fine. The help documentation explains:
Clearance Pass Stepover
Only used when a V-Bit tool is being used to rough machine at multiple Z levels down to a specified flat depth. This stepover can be much larger than the Final Pass Stepover because the tool is only rough machining material away. Increasing the Clearance Pass Stepover will reduce the machining time, but you must be careful to ensure it is not too great for the material being cut.
[Final Pass] Stepover
The distance the cutter moves over when finish machining and is usually set to be a relatively small distance to produce a smooth surface finish on the job.
Therefore, if you want the flat areas to be smoother using the engraving tool you should set the [Final Pass] Stepover to be less than half of the flat diameter. Obviously this will increase machine time. This is where you have to decide if you want to save time by using an additional tool for clearing the flat areas, or if you are willing to wait longer to avoid a tool change.
- Randall Newcomb
10 fingers in, 10 fingers out, another good day in the shop
10 fingers in, 10 fingers out, another good day in the shop