V-Carve pro ver 8 problem

[steve_g]

I’m having an issue with VCP8… When I do a V-carve with a lot of piercings, I limit my depth of cut so I don’t destroy my spoilboard. Then, so I don’t have to spend the time V-carving away the waste areas, I tell the software to use a flat clearance tool, but don’t actually run that toolpath because those waste parts will just fall off when the part is removed from the machine… This used to work just fine but now, noticed it first today, The V.carve toolpath doesn’t cut the waste areas to a complete V, but leaves a flat area on it. This is causing missteps during the v-carving due to interference with the bit. The CMT bit has an area above the sharpened cutting area that lands up rubbing on that flat spot.
My Question…
Have I missed something in the setup?
SG

[Brady Watson]

Steve,
How deep are you cutting? That tool has a max CEL/LOC of .4375" - so if you cut deeper than this, regardless of pass depth, it will bite into the sides.

You may want to pick up one of these bad boys: Onsrud 37-82 (http://ballewsaw.com/onsrud-37-82-double-flute-carbide-tipped-lettering-bits.html) 1" dia, 60 deg, .85" LOC.

-B

[steve_g]

Brady…
I’m cutting .75” deep, I thought that VCP would step any size v-bit down any depth. In fact I routinely V-carve bench miter joints 3” deep!
SG

[Brady Watson]

Yes, Steve....but you did the miter joint with a completely different bit, with different angle and grind.

Take that bit and cut with it .375" deep - just a machine along vector (or keypad + arrow keys). Observe the cut profile. Now, cut it again but .5" deep. You will see the side of the bit biting in. This will be true for any depth greater than .4375", because that is how deep the tool is ground. The Onsrud I recommended will get you .85" before you run into that.

The outer perimeter of your area will be 'stepped' and the inside will be like you'd expect. This is 100% the result of the grind of the bit. No setting in VCP or Aspire can fix this issue.

-B

[steve_g]

I understand what you’re saying, BUT, my project isn’t machined along a vector… It’s a true “V-carve” toolpath.

FYI. I use a 1.5” 90° V-bit on my benches, I use a v-carve toolpath based on a rectangle large enough to get the results I want.
SG

[srwtlc]

Steve, are you setting a start depth other than 0? It looks like what one gets when doing a vcarve inlay and the chosen bit doesn't have the diameter to handle the depth.

[Brady Watson]

Steve/Scott,
That's the only way I can get it to come up with that ridge - by setting the start point below the surface.

If you post the file, one of us can verify what is going on using VCP8.

-B

[steve_g]

https://drive.google.com/file/d/0B8GtiBWUjRyRYmdUVzhMYUtOeGs/view?usp=sharing
Here’s the file… remember, I toolpathed like I was using a flat area clearance but don’t actually run that toolpath.

Thanks!
SG

[Brady Watson]

Steve,
Thanks for the file. I don't think there isn't any way to do what you want without jumping through some hoops or paying the time penalty.

If you eliminate the roughing pocket, you get the stepped islands.

If you keep the flat depth and don't check to use a roughing tool (just the 60v), then you are spending a lot of time machining.

The quick & dirty solution may be to do a little bit of file manipulation. Do a regular V-carve TP without the flat and then change all of the negative values below your .77 threshold to equal .77 - this is a pain, but there is no other way I can think of at the moment to do what you want to do. Excel may be easiest with this...AND if you do choose this option, break up the toolpath so that the deepest areas wind up in their own toolpath so that it is easier to edit.

How many of these are you making?

-B

[Brady Watson]

One more thing that might not be too painful...ShopBot Labs File modifier (http://www.shopbottools.com/LabFiles/filemodifier.htm). This is one of Bill Young's hidden gems.

Save out a regular old v-carve toolpath & make sure there aren't any circle or arcs commands (there should not be for a v-carve). Run SB3 Preview and note the max depth that the tool goes. Then open up the modifier.

In this case, I elected to modify the Z, IF the Z value was below -0.77 tbe n add .94" to it. This will result in some air cutting, but it will not gouge the bed.

Try it for yourself.

-B

[steve_g]

Thanks Brady…
I’m only making five of these… It’s a technique I’ve used for years and then suddenly I’m bit on the butt with this one! I thought it strange that I was missing steps so I’d start it over with slightly different settings… I demonstrated the definition of insanity by repeatedly trying the same thing expecting different results!
Likely the good folks at Vectric were trying to save some cutting time by not finishing the cuts of areas they thought wouldn’t be there if/when used as designed!
It used to work, something changed with a version/update and I missed the white paper…
Thanks again for verifying that I hadn’t messed up a setting somewhere!

To the Folks at Vectric… toolpathing the removal of the waste is great for rendering purposes, but in real life, time is saved by not actually running that toolpath when piercing the material!
SG

[steve_g]

File modifier…
Ok, I really missed that option… I’ll give it a try!
Thanks!
SG

[steve_g]

Whoops! Win 10 doesn’t like the file modifier…

SG

[Brady Watson]

That's just a COM component missing...pretty standard VB stuff. I am surprised 10 doesn't have it. You may want to download it and throw it in System32. Make sure you use RegSrvr. See here (http://www.sevenforums.com/bsod-help-support/59463-comdlg32-ocx.html).

I ran the same toolpaths in PW2.5 and VCP8.024 and I cannot see a difference between the v-carve toolpath by itself, with pocket checked, but not used/simulated. They pretty much look identical.

-B

[scottp55]

Steve,
Just for kicks and giggles I plugged a .5"downcut in, instead of your .125, and only got an increase of 5 minutes on the VCarve portion, with only a 5 minute (clearance) time.
I'm probably missing something.
Just thinking.
scott

[steve_g]

Brady…
An interesting side by side comparison! What it tells me is that, as reported, I’m crazy! All I can figure is that in the past I’ve always done this type of project on my Alpha and this one was done on a friend’s standard… The alpha likely powers through the islands while the standard misses steps.

Scott…
It’s true, I’ll do most anything to avoid a tool change!

Thanks all for your patience with me!

SG

[Brady Watson]

What it tells me is that, as reported, I’m crazy!


It's OK, Steve. You're among friends! ;)

-B

[scottp55]

:)
ALMOST as bad as you!
Tried to design a button last week using JUST a Whiteside .5D .25R point cutting roundover....IF you squint real hard it looks like an Owl:)
scott