Outlines around letters

[grubby65]

I carved my first sign and I am having issues with the letters. As you can see there was an outline around the letters. I was using V-Carve/Engraving Toolpath. The bits used were a .25" End Mill for the flat area and a .125" Ball Nose for around the letters. The flat area had a depth of .25". I was wondering if someone could help me figure out what I might have done wrong. I rechecked the zero (surface of the wood) on the .125" ball nose and it checked out fine. Any help would be appreciated.
Thanks

[TReischl]

Grubby, one of the best things you can do is learn how to attach a file to your posts or if they are too big for that putting them in something like DropBox or OneDrive.

What happens is people will need to speculate on just how you really set things up, whether or not your machine is losing steps, the bit is slipping in the collet, etc.

BTW, congratulations on building your machine! Over the years I have done quite a few WoodSmith projects.

[garylmast]

I was having that problem, which was caused when I zero the mill to the wood, one would recess slightly in to the wood more than the other, making it off by a few thousands. How I solved it was I have a metal plate I lay on top of the wood, and then when I zero it, I will put the thickness of the plate in the Zero Column. That way I know all the mills are zero at the same.

Gary

[grubby65]

Welcome sign (2).zip

(1.22 MiB) Downloaded 81 times

I am actually using V-VarvePro, so I guess I posted this in the wrong area. Sorry about that. I have attached the program file. After looking at it I see the outline around the letters, is this something VCarve automatically does?

[Adrian]

Can be lots of different reasons none of which are to do with the software. The Z-zero can be fractionally off when changing bits, the wood can expand/move, the different type of bit (ball nose versus spiral endmill versus bottom cutting end mill etc) can all cut the material slightly differently.

As an aside I would weld the main text so the vectors flow rather than relying on the bit not going into the gaps.

[grubby65]

Can be lots of different reasons none of which are to do with the software. The Z-zero can be fractionally off when changing bits, the wood can expand/move, the different type of bit (ball nose versus spiral endmill versus bottom cutting end mill etc) can all cut the material slightly differently.

As an aside I would weld the main text so the vectors flow rather than relying on the bit not going into the gaps.

Thanks for your response. I'm new to this, so if you would, could expand on the "weld the main text"?

[dealguy11]

The problem shows up in the preview, so it's not entirely a machine issue. Part of it, I think, is from using a ballnose bit in a v-carve toolpath, which doesn't make a lot of sense. Try again with the same 2 bits, but make it a pocket toolpath instead.

[grubby65]

Thank you so much for your reply. Like I said I'm new to this, I guess I thought the V-Carve engraving was something special for lettering. I did as you suggested and ran it just using profile with two bits and it worked out perfectly. I will try it tonight. Once again thanks for your help.

[Leo]

There are a few things I see.

1 - Welding
Welding will work when the letters are slightly overlapping like they are in the word WELCOME on the last 2 letters - M & E. Move the letters ELCOM - so those letters overlap like the last 2 letters. After the letters are in the location of overlapping - WELD. There are some really nice tutorials on the WELD command

2 - Toolpath
Don't use the Vcarve/Engraving tool path. Also first don't use a ball end mill with Vcarve tool path, and second don't use a ball end mill for your project. This is just a pocketing toolpath. You CAN use a straight 1/8 and a straight 1/4 end mills and use the POCKET toolpath.

Generally, when I do this I will set my 1/8 cutter just a TAD higher on the "Z" - like .005-.008. This way I can run the tool path on the 1/8 cutter and it "should" leave a little raised step. I measure that step and reset the 1/8 cutter on "Z" and rerun the toolpath until it matches nicely. You can sneak up nicely this way.

Another thing than can be done on the 1/8 cutter is the set it to slightly smaller diameter than it actually is. That will make it cut a tiny amount more on the perifery of the letters and clean up the sides of the letters a bit. On the second run around I will cut full depth.

This is probably about as clear as mud, but it works.

[grubby65]

Your comments were very informative and I will give them a try. I'm currently above 45 degrees on the learning curve right now. Thanks for your help.

[Leo]

The curve gets steeper and steeper the further you go.