Final Pass how to

This forum is for general discussion regarding VCarve Pro

Final Pass how to

Postby mikenbrenda » Thu Jun 20, 2019 5:59 pm

when i always hear someone say "I Ran a Final Pass" what does that exactly mean?, is there a way to run a final pass without going thru the whole tool path Code again let's say? like in VCarve Pro, I see it like on a Profile Path option, like take off .005 or something, but what about a Vcarve let's say...like just one pass at the bottom of the depth so to speak if i am saying that right..??
mikenbrenda
 
Posts: 28
Joined: Thu Nov 22, 2018 6:46 pm
Model of CNC Machine: Shapeoko 3 XXL

Re: Final Pass how to

Postby dealguy11 » Thu Jun 20, 2019 6:11 pm

Yes, usually when people talk about the "final pass" option they're usually talking about that checkbox in the Profile toolpath.

There are other ways to take a final pass. In your v-carve example, if you're taking multiple passes because your machine can't power through all that material in one pass, then the last one of those passes is sort of automatically a "final pass" because the tool will be touching the side of the cut top to bottom on that pass. If you want to redo that last pass just to make sure everything is cleaned up, you can copy the toolpath, but change the depth of cut for the tool to the maximum depth of the profile or greater by editing the tool for just that toolpath.

If you want to create a final pass for a profile toolpath without using the option on the toolpath screen (for example, maybe you want to cut all the parts down to all but the last .01" to leave an onion-skin to hold the parts in place, then go back and cut the onion skin to cut them out with less possibility of parts moving, and you want to cut the onion skin for all parts in one toolpath rather than one part at a time), then you can just create another profile toolpath with the start depth of however deep the first profile cut went, and a depth of cut of .01" to cut away the onion skin.

Basically you can set up your toolpaths with cut depths and offsets to create any sequence of cuts and final cuts you want.
Steve Godding
D&S Artistic Woodworking http://www.dsartisticwood.com
User avatar
dealguy11
Vectric Wizard
 
Posts: 1394
Joined: Tue Sep 22, 2009 9:52 pm
Location: Henryville, PA
Model of CNC Machine: Anderson Selexx 510

Re: Final Pass how to

Postby tomgardiner » Thu Jun 20, 2019 8:04 pm

Just so dealguy's instructions are totally clear, the start depth is set in the top field of a toolpath menu. Be careful once using it though as the next time you set up a toolpath of the same style (pocket for instance) then the start depth value will be the default. It can ruin your mood.
tomgardiner
Vectric Wizard
 
Posts: 354
Joined: Thu Oct 02, 2014 1:49 pm
Model of CNC Machine: FMT Patriot 4 x8

Re: Final Pass how to

Postby TReischl » Fri Jun 21, 2019 12:41 pm

mikenbrenda wrote:when i always hear someone say "I Ran a Final Pass" what does that exactly mean?.....


What they should be saying is they ran a FINISH pass. There is always a FINAL pass, it is the last pass. In machining everyone understands that FINISH pass means a light pass to clean up the cut.
http://www.tedreischl.com

Low Profile CNC Router Vise
User avatar
TReischl
Vectric Wizard
 
Posts: 2719
Joined: Thu Jan 18, 2007 6:04 pm
Location: Leland NC
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset

Re: Final Pass how to

Postby mikenbrenda » Fri Jun 21, 2019 1:30 pm

I guess maybe i should have said finish Pass then, is there a way to run a "Finish Pass" then in Vcarve a final light pass? without running the whole code? like you a can tell it to run the last part or final pass of the code?
mikenbrenda
 
Posts: 28
Joined: Thu Nov 22, 2018 6:46 pm
Model of CNC Machine: Shapeoko 3 XXL

Re: Final Pass how to

Postby Adrian » Fri Jun 21, 2019 1:44 pm

mikenbrenda wrote:I guess maybe i should have said finish Pass then, is there a way to run a "Finish Pass" then in Vcarve a final light pass? without running the whole code? like you a can tell it to run the last part or final pass of the code?

Depends which toolpaths you're talking about.
User avatar
Adrian
Vectric Archimage
 
Posts: 9371
Joined: Thu Nov 23, 2006 2:19 pm
Location: Surrey, UK
Model of CNC Machine: ShopBot PRS Alpha 96x48

Re: Final Pass how to

Postby mikenbrenda » Fri Jun 21, 2019 1:50 pm

The pocket tool paths are no problem, it is teh Vcarve tool paths that does nto seem to have that options. as mentioned before in my original thread..
mikenbrenda
 
Posts: 28
Joined: Thu Nov 22, 2018 6:46 pm
Model of CNC Machine: Shapeoko 3 XXL

Re: Final Pass how to

Postby Adrian » Fri Jun 21, 2019 2:22 pm

Sorry, always get confusing when people talk about VCarve rather than V-carve. One is the name of the software and the other is a toolpath. I should have spotted that. The first reply to your post explains how to do it with that toolpath. There's no option as a finishing pass in that context is a different thing to a final pass although they are pretty much the same thing in a profile toolpath.
User avatar
Adrian
Vectric Archimage
 
Posts: 9371
Joined: Thu Nov 23, 2006 2:19 pm
Location: Surrey, UK
Model of CNC Machine: ShopBot PRS Alpha 96x48

Re: Final Pass how to

Postby TReischl » Fri Jun 21, 2019 9:37 pm

I just finished a larger V carve (looks like chip carving that Wayne Barton teaches) in walnut. I used a brand new cutter but the problem is that no matter what you do sometimes the cutter is cutting uphill against the grain. Lathe guys know what I am talking about, you never cut uphill into the grain, or a guy who uses a hand plane understands it very well, he looks to see that the cutter is not going against the grain. Anyway, it resulted in a case of the nasty fuzzies on some of the cuts, a lot of the cuts actually.

Soooo, I gave it a coat of sanding sealer, let it dry real well and then ran a second pass to the same depth. What I did was tell the software that my cutter could go deeper than the deepest cut. That way it did not waste time roughing out air. Came out very nice.
http://www.tedreischl.com

Low Profile CNC Router Vise
User avatar
TReischl
Vectric Wizard
 
Posts: 2719
Joined: Thu Jan 18, 2007 6:04 pm
Location: Leland NC
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset

Re: Final Pass how to

Postby dah79 » Sat Jun 22, 2019 1:17 pm

TReischl wrote:Soooo, I gave it a coat of sanding sealer, let it dry real well and then ran a second pass to the same depth. What I did was tell the software that my cutter could go deeper than the deepest cut. That way it did not waste time roughing out air. Came out very nice.


Interesting process. How do you tell your cutter to go deeper than the deepest cut? What kind of toolpath were you running? Thanks
Dave
dah79
Vectric Wizard
 
Posts: 332
Joined: Thu May 14, 2015 12:23 am
Location: Bemidji, MN
Model of CNC Machine: FLA Saturn 4x4

Re: Final Pass how to

Postby gkas » Sat Jun 22, 2019 3:14 pm

You can edit the tool in your toolpath; change it's properties without changing the tool parameters in the database. It's an edit for that toolpath only.

Normally, you may have the DOC set to 0.15 inches on a 0.25 bit. But using this setting for a cleanup pass results in a lot of air cutting. If your pocket is 0.3 inches, change the DOC to 0.4 inches. Rerunning the pass results in only one clearance pass.
User avatar
gkas
Vectric Wizard
 
Posts: 394
Joined: Sun Jan 01, 2017 3:39 am
Location: Southern California
Model of CNC Machine: Aspire, Axiom AR8 Pro+, Axiom 4.2W Laser

Re: Final Pass how to

Postby TReischl » Sat Jun 22, 2019 8:46 pm

dah79 wrote:
TReischl wrote:Soooo, I gave it a coat of sanding sealer, let it dry real well and then ran a second pass to the same depth. What I did was tell the software that my cutter could go deeper than the deepest cut. That way it did not waste time roughing out air. Came out very nice.


Interesting process. How do you tell your cutter to go deeper than the deepest cut? What kind of toolpath were you running? Thanks


What GKGAS said!
http://www.tedreischl.com

Low Profile CNC Router Vise
User avatar
TReischl
Vectric Wizard
 
Posts: 2719
Joined: Thu Jan 18, 2007 6:04 pm
Location: Leland NC
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset

Re: Final Pass how to

Postby mikenbrenda » Mon Jun 24, 2019 3:45 pm

That's weird so you are saying just by editing the pocket tool path to a .01 difference let's say it will skip all of the air passes and just do one pass ? not the rest? that would be cool
mikenbrenda
 
Posts: 28
Joined: Thu Nov 22, 2018 6:46 pm
Model of CNC Machine: Shapeoko 3 XXL

Re: Final Pass how to

Postby dealguy11 » Mon Jun 24, 2019 5:18 pm

The general rule is that if the depth of cut for the tool is less than the total depth required for the toolpath, then you will get multiple passes. If the depth of cut for the tool is greater than the depth of the toolpath then you'll get one pass.
Steve Godding
D&S Artistic Woodworking http://www.dsartisticwood.com
User avatar
dealguy11
Vectric Wizard
 
Posts: 1394
Joined: Tue Sep 22, 2009 9:52 pm
Location: Henryville, PA
Model of CNC Machine: Anderson Selexx 510

Re: Final Pass how to

Postby TReischl » Tue Jun 25, 2019 1:09 pm

mikenbrenda wrote:That's weird so you are saying just by editing the pocket tool path to a .01 difference let's say it will skip all of the air passes and just do one pass ? not the rest? that would be cool


Noooo, that is not what I said.

Let's say I have a 1.00 dia 90 degree V Bit. The deepest it can cut in a single pass is .500.

So if my deepest cut in the work is .375 and I set up the tool to allow .500 in a single pass in depth of cut then the program will cut to full depth eliminating clearance passes.

When doing things like this the Edit button in the choose Tool panel is your friend. When you Edit a tool setting it does not change it in the database, just for that toolpath.
http://www.tedreischl.com

Low Profile CNC Router Vise
User avatar
TReischl
Vectric Wizard
 
Posts: 2719
Joined: Thu Jan 18, 2007 6:04 pm
Location: Leland NC
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset

Next

Return to VCarve - General

Who is online

Users browsing this forum: No registered users and 22 guests