Can I use an open vector for tool path

This forum is for general discussion regarding VCarve Pro
dehaan
Posts: 13
Joined: Thu Nov 29, 2018 12:07 am
Model of CNC Machine: CNC SHARK II

Can I use an open vector for tool path

Post by dehaan »

I am trying to undercut the perimeter of a pocket using a flat undercutting router bit. To avoid cutting down directly through the finished edge I would like to create a cutting path to follow a polyline. This would allow mw to drop into the center of an existing pocket, set my depth run around the perimeter of the existing pocket and then return to center before raising the bit.
Any suggestions? I seem to be stumped.

User avatar
highpockets
Vectric Wizard
Posts: 3667
Joined: Tue Jan 06, 2015 4:04 pm
Model of CNC Machine: PDJ Pilot Pro

Re: Can I use an open vector for tool path

Post by highpockets »

Google Vectric Keyhole.
John
Maker of Chips

User avatar
Adrian
Vectric Archimage
Posts: 14544
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: Can I use an open vector for tool path

Post by Adrian »

You can run a profile cut on an open vector. It can be on the line, to the right of it or to the left of it. What is right or left is determined by where the start node of the line is. Imagine walking down the line starting from the start and you'll understand what the left and right means.

To get the bit to move to the edge of the pocket you can either extend the vector so it starts and ends in the middle of the pocket but that will only work if the bottom of the pocket is the same depth as the intended depth of the slot. Otherwise you will need to use the lead-in and lead-out feature of the toolpath with a ramp set.

Be sure to double and triple check all the plunges and retracts in the preview before running the toolpath for real.

dehaan
Posts: 13
Joined: Thu Nov 29, 2018 12:07 am
Model of CNC Machine: CNC SHARK II

Re: Can I use an open vector for tool path

Post by dehaan »

When I try to use a keyhole approach the profile toolpath does not seem to want to start at 0.4 inches and insists on cutting through the entire work piece - even when I insert the starting depth at 0.4 and finish depth at 0.401. If I try to use a pocket approach it does not like an open vector.

User avatar
Adrian
Vectric Archimage
Posts: 14544
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: Can I use an open vector for tool path

Post by Adrian »

Can you attach the file to show what you're doing as I'm not really following what you mean by the 0.4" bit. Did you follow the steps in my previous post? There's no need to program it like a keyhole as (from what you said in the 1st post) you're cutting a continous line starting and ending in the same place but not going back on itself.

It definitely won't work at all with a pocket cut as that is 100% the wrong toolpath to use.

User avatar
mtylerfl
Vectric Archimage
Posts: 5865
Joined: Thu Jan 29, 2009 3:54 am
Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha
Location: Brunswick, GA

Re: Can I use an open vector for tool path

Post by mtylerfl »

Don’t forget to subtract the Start Depth amount from your total Depth amount to avoid cutting too deep (as you described).

As always, including a file along with questions, really helps to save time “guessing” what’s going on.
Michael Tyler

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC

User avatar
Leo
Vectric Wizard
Posts: 4082
Joined: Sat Jul 14, 2007 3:02 am
Model of CNC Machine: 1300 x 1300 x 254 Chinese Made
Location: East Freetown, Ma.
Contact:

Re: Can I use an open vector for tool path

Post by Leo »

If doing an undercut - be sure to have a start position at the cutting level then cut into the undercut - move along the undercut profile and at the end - have a move to move the cutter out of the undercut BEFORE you retract the cutter.
Imagine the Possibilities of a Creative mind, combined with the functionality of CNC

dehaan
Posts: 13
Joined: Thu Nov 29, 2018 12:07 am
Model of CNC Machine: CNC SHARK II

Re: Can I use an open vector for tool path

Post by dehaan »

OK Here goes. I will try and find out how to attach my project file in VCARVE.
To clarify, I am essentially trying to cut a slot around the four sides of a pocket which I have created. Wood thickness is 0.75 and the pocket depth is 0.4.
I understand that an additional pocket cut is out of the question for this part of the project.
What I have done is try a profile cut using a polygon created to allow for the beginning and end point of the profile to be in or near the center of the existing pocket. When I insert Start depth of 0.4 and End depth of 0.401 the profile insists on cutting through the entire 0.75 stock. The bit I am trying to use is a 1.25" Outer Diameter flush cutting [upper bearing] slot cutter with a 1/4" shaft and a cutting depth of 1/8" and usable cut radius of 5/16" - of which I want something like 3/16". Essentially, running an undercut [1/8" deep and 3/16" wide] completely around the perimeter of the pocket. Additionally, I would like to cut a similar slot along the upper top edge of the handle to allow an insert [acetate sheet] to be dropped into the pocket. Probably a relatively simple solution but I am a novice. Thanks for your help - I seriously appreciate it.
Attachments
slot1.crv
slotted tap handle
(116.5 KiB) Downloaded 86 times

User avatar
Adrian
Vectric Archimage
Posts: 14544
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: Can I use an open vector for tool path

Post by Adrian »

Sounds like you've set the cut depth to be 0.401 when you need it to be 0.01 instead. At the moment you would be starting at 0.4 and then cutting 0.401 from that point with the settings you describe.

dehaan
Posts: 13
Joined: Thu Nov 29, 2018 12:07 am
Model of CNC Machine: CNC SHARK II

Re: Can I use an open vector for tool path

Post by dehaan »

You are absolutely right. I reset the cut depth to 0.001 after a start depth of 0.4
I then did some manipulating of the open vector [for the slot profile] for the slot cut using node edit and got the start and end were I wanted it.
I will still need to do some careful calculating to get the slot where I want it.
Thanks again - you folks are a great help!

User avatar
Leo
Vectric Wizard
Posts: 4082
Joined: Sat Jul 14, 2007 3:02 am
Model of CNC Machine: 1300 x 1300 x 254 Chinese Made
Location: East Freetown, Ma.
Contact:

Re: Can I use an open vector for tool path

Post by Leo »

I am having a really hard time trying to understand what you are trying to do.

Screen shots of what you are having problems with would be a GREAT help.

vectric does not display toolpath of undercuts. It will appear as though you are cutting the entire depth even though you are trying to make a slot around the perifery of a pocket. In that case there is no solution, but in reality it is ONLY in the preview, not in the actual cutting. To some point there is a point where you gotta have a little faith.

BUT

I am only guessing at what you are seeing.

Show us the cutter - take a pic and post it
Show us what you are seeing on the screen
Make a pencil and paper sketch - take a pic - post it

We just need to be able to see.
Imagine the Possibilities of a Creative mind, combined with the functionality of CNC

User avatar
mtylerfl
Vectric Archimage
Posts: 5865
Joined: Thu Jan 29, 2009 3:54 am
Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha
Location: Brunswick, GA

Re: Can I use an open vector for tool path

Post by mtylerfl »

Leo,

Visit this post for more detail...

http://forum.vectric.com/viewtopic.php? ... ot#p226043

...and visit this post for the type of cutter being used:

https://ballewsaw.com/shop-by-brand/sou ... saw-blades
Michael Tyler

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC

User avatar
Leo
Vectric Wizard
Posts: 4082
Joined: Sat Jul 14, 2007 3:02 am
Model of CNC Machine: 1300 x 1300 x 254 Chinese Made
Location: East Freetown, Ma.
Contact:

Re: Can I use an open vector for tool path

Post by Leo »

Thank you Michael

I am very familiar with slot cutters - but what confused me is that Dehaan mentioned that he is using ---("The bit I am trying to use is a 1.25" Outer Diameter flush cutting [upper bearing] slot cutter with a 1/4" shaft and a cutti")--- If you are POSITIVE he is using the cutter you linked to then I am OK with that.

Also - I was not aware of other threads on the same subject. That just adds more confusion.

I'm afraid that me posting is adding even "more" confusion.
Imagine the Possibilities of a Creative mind, combined with the functionality of CNC

User avatar
mtylerfl
Vectric Archimage
Posts: 5865
Joined: Thu Jan 29, 2009 3:54 am
Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha
Location: Brunswick, GA

Re: Can I use an open vector for tool path

Post by mtylerfl »

Hi Leo,

I’m not positive the correct bit is being used, but we all hope so!

It certainly would have been best for continuity and info to keep posting in the very first thread (instead of at least three separate threads). Oh well!
Michael Tyler

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC

dehaan
Posts: 13
Joined: Thu Nov 29, 2018 12:07 am
Model of CNC Machine: CNC SHARK II

Re: Can I use an open vector for tool path

Post by dehaan »

Will try and add some images.
Things came out pretty well and my perimeter slot worked after a couple of tweaks
Thanks for the help
Attachments
KAMB.jpg
semi fin.jpg
slot bit.jpg

Post Reply