Help with Pockets Please

This forum is for general discussion regarding VCarve Pro
Post Reply
RobH063
Vectric Craftsman
Posts: 106
Joined: Sun Jan 17, 2016 4:19 pm
Model of CNC Machine: 1000mm Xcarve
Location: Jamestown, New York

Help with Pockets Please

Post by RobH063 »

I want to make a circular pocket that's precise and .25" deep but I get this vertical mark where the end mill plunges in as shown in the drawing. The pocket is being created with two passes at .125" depth per pass using a .25" down cut end mill. I assume they are deflection marks from plunging in and out at the same location, and the torque created once the cut begins. It makes no difference with speeds and feeds as I've adjusted them numerous times in an attempt to solve this problem. Will using the Ramp feature eliminate this? If it were a Profile cut, I could use the Lead in/out feature but that's not an option with a Pocket cut. Or do I have to cut the pocket and use a positive Pocket Allowance and then do a Profile finish pass using the Lead in/out feature? Then there's the issue of the Lead in/out not starting from within the pocketed circle. It wants to start from outside of the circle and that would ruin the pocket. I don't know how to change the Lead in/out starting point so the pocket wouldn't be ruined. Any help with that as well would be greatly appreciated. Thank you in advance.
PocketMark.jpg

User avatar
Adrian
Vectric Archimage
Posts: 14546
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: Help with Pockets Please

Post by Adrian »

When you create the profile cut to get the leads make sure that the cut is set to be inside the vector not outside. That way the leads will be created on the scrap inside the pocket. Finish off with a pocket.

See here - http://forum.vectric.com/viewtopic.php?f=2&t=28337

RobH063
Vectric Craftsman
Posts: 106
Joined: Sun Jan 17, 2016 4:19 pm
Model of CNC Machine: 1000mm Xcarve
Location: Jamestown, New York

Re: Help with Pockets Please

Post by RobH063 »

Thank you Adrian. One last question regarding Lead ins and outs. Many times with choosing both Lead ins and Outs I get a warning telling me about the gouging and that the software has reduced or eliminated one or more Lead Ins or Outs. Sometimes both are removed. Is there a way to change where they start so they don't have to be removed? Sometimes the software chooses locations on where to start a cut so a Lead in/out can't be used.

RobH063
Vectric Craftsman
Posts: 106
Joined: Sun Jan 17, 2016 4:19 pm
Model of CNC Machine: 1000mm Xcarve
Location: Jamestown, New York

Re: Help with Pockets Please

Post by RobH063 »

Disregard last post. I figured it out. Thank you

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: Help with Pockets Please

Post by Leo »

That's an age old issue in metal cutting.

Solution is - curved ramp in and curved ramp out.

No you cannot do it with pocketing, BUT it still CAN be done.

1) do the pocketing but leave ample material for finishing.
2) do a profile cut with spiral ramp in and spiral ramp out

Stack both toolpaths in one output g-code file.
Imagine the Possibilities of a Creative mind, combined with the functionality of CNC

User avatar
martin54
Vectric Archimage
Posts: 7339
Joined: Fri Nov 09, 2012 2:12 pm
Model of CNC Machine: Gerber 48, Triac PC, Isel fixed gantry
Location: Kirkcaldy, Scotland

Re: Help with Pockets Please

Post by martin54 »

I normally do what Leo has suggested, cut the pocket smaller than it needs to be & then profile cut using a spiral ramp, both toolpaths with the same tool & output together so as soon as the pocket is cut the machine moves straight on to the profile cut :lol: :lol:

4DThinker
Vectric Wizard
Posts: 1701
Joined: Sun Sep 23, 2012 12:14 pm
Model of CNC Machine: CNC Shark Pro, Probotix Meteor 25" x 50"

Re: Help with Pockets Please

Post by 4DThinker »

If you choose the raster option with your pocket toolpath you can set it to do a profile pass as the last pass. This will do exactly what has been suggested previously, but all in the same toolpath.

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: Help with Pockets Please

Post by mtylerfl »

4DThinker wrote:If you choose the raster option with your pocket toolpath you can set it to do a profile pass as the last pass. This will do exactly what has been suggested previously, but all in the same toolpath.
+1
Michael Tyler

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC

RobH063
Vectric Craftsman
Posts: 106
Joined: Sun Jan 17, 2016 4:19 pm
Model of CNC Machine: 1000mm Xcarve
Location: Jamestown, New York

Re: Help with Pockets Please

Post by RobH063 »

4DThinker, if using the Raster option, would you eliminate the pocket allowance because there would be no need to do a finish pass?

4DThinker
Vectric Wizard
Posts: 1701
Joined: Sun Sep 23, 2012 12:14 pm
Model of CNC Machine: CNC Shark Pro, Probotix Meteor 25" x 50"

Re: Help with Pockets Please

Post by 4DThinker »

RobH063 wrote:4DThinker, if using the Raster option, would you eliminate the pocket allowance because there would be no need to do a finish pass?
I only use an allowance on pockets for joinery that has two parts that need to fit precisely. So yes, with the raster option and last-pass profile I don't use an allowance. I also try and set the raster direction to run parallel with the wood grain.

4D

RobH063
Vectric Craftsman
Posts: 106
Joined: Sun Jan 17, 2016 4:19 pm
Model of CNC Machine: 1000mm Xcarve
Location: Jamestown, New York

Re: Help with Pockets Please

Post by RobH063 »

Ok, Thank you. I'll give it a try

User avatar
Adrian
Vectric Archimage
Posts: 14546
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: Help with Pockets Please

Post by Adrian »

I suggested a few years ago using raster toolpath with a final pass on the ShopBot forum for this issue but I was told at the time it is inferior to the offset toolpath in aluminium in terms of finish. Is that not the case? I'd like to know for future reference.

In wood and plastic I rarely use the offset strategy as I much prefer the raster option for the extra control.

RobH063
Vectric Craftsman
Posts: 106
Joined: Sun Jan 17, 2016 4:19 pm
Model of CNC Machine: 1000mm Xcarve
Location: Jamestown, New York

Re: Help with Pockets Please

Post by RobH063 »

That's good to know Adrian. I may never use anything other than wood and maybe plastic but not anytime soon. I'll be trying the raster option later today and see what happens.

Post Reply