Marks left in tab locations, any suggestions appreciated.
Just noticed this on recent carve
What CAM software are you using? If you are using anything from Vectric, you may have more luck with 3D tabs.
Vetric V Carve pro up to date ver 11.
@Bill In the tabs box, there are 3 choices.One of them is 3D tabs. The benefit of them is that the machine does not stop to go straight up on one side of a tab, then stop again to go straight down. The 3D tabs are ramped on both sides, so not only do they allow the machine to keep moving, but they seem to reduce or eliminate the registration marks that you are getting.
If you try them please report back on your experience.
1 Like
I agree with @gwilki, use the 3d tab choice.
Anytime your tool-path movement stops/dwells in one spot, then restarts, you will have tool deflection because of the cutting action, which will leave a mark/rat bite.
Please note that 3d tabs should be long enough, and thick enough, to support your project when cut out. A 3d tab does not have the same cross-section as a square tab, so just be aware of that design feature. Don’t go to thin and too short.
The tool deflection can be caused by equipment/part clearances, worn parts, lose running clearances in the router/spindle, tool extended too far out from collet, etc.
Most of these issues, if properly managed thru the tool-paths, will still give you a good finished project.
I also use the lead in function to eliminate/reduce that same issue when starting the cut.
Just keep experimenting.
2 Likes
Thanks to all for suggestion with checking the 3D option, @RustyR could you please provide what settings for leads you typically use?
2 Likes
@Bill, I typically use .125" high X .375-.500" long, depending on tab location access and material type and thickness.
Tips:
- position/locate tabs in straight sections, or long arc’d outside curves (not on inside curves).
- position/locate tabs on the cut line in areas that will still be supported by the clamps. Do not place tabs in sections that will become loose when bit cuts thru.
- place tabs in areas that allow good access to cut the tabs, as well as, to sand them to finished outline .
- thru experimentation you will discover how small of a tab you can use. I tend to go on the thicker and longer design because I also utilize the tabs to help with some post machining work-piece finishing processes.
- I use Vectric software, so make sure the tabs are in-place when you run your tool-path simulation. Many times I though I had properly located the tabs, but they weren’t there when I ran the tool-path simulation. Reply on that simulation to proof your tool-paths. It works amazingly.
1 Like
@RustyR Good explanation, Rusty. I think that Bill was interested in your leads settings, too. 
OK, lead-in and lead-out settings:
- generally, for in and out, I use at least one inch diameter arcs with a length of approx .500"/side, with an over-lap of at least .06" - .100"
- the above dimensions will depend on your work-space/material specs related to your finished work-piece. As long as your tool is at cutting depth prior to moving to your finish outline size then you will be OK. The bit will now be under tool cutting pressure.
Remember to review/clarify using the tool-path simulation. Trust what you see and adjust accordingly, if neccesary. - you can also adjust where the lead-in starts in relationship to your finishing outline cut. Play with that so you have good access for the lead-in/lead-out. I can’t remember how to adjust that but it is in relation to where your tool will start cutting, which can be adjusted.
Note: I rarely use the ramp-in/out function, but it also has it’s purpose.
1 Like
Thanks again for the help and info, very much appreciated
Bill