Help with Pockets Please

This forum is for general discussion regarding VCarve Pro

Help with Pockets Please

Postby RobH063 » Fri Oct 27, 2017 2:48 pm

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
RobH063
Vectric Apprentice
 
Posts: 83
Joined: Sun Jan 17, 2016 4:19 pm
Location: Jamestown, New York
Model of CNC Machine: 1000mm Xcarve

Re: Help with Pockets Please

Postby Adrian » Fri Oct 27, 2017 2:57 pm

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 - viewtopic.php?f=2&t=28337
User avatar
Adrian
Vectric Archimage
 
Posts: 7422
Joined: Thu Nov 23, 2006 2:19 pm
Location: Surrey, UK
Model of CNC Machine: ShopBot PRS Alpha 96x48

Re: Help with Pockets Please

Postby RobH063 » Fri Oct 27, 2017 3:37 pm

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 Apprentice
 
Posts: 83
Joined: Sun Jan 17, 2016 4:19 pm
Location: Jamestown, New York
Model of CNC Machine: 1000mm Xcarve

Re: Help with Pockets Please

Postby RobH063 » Fri Oct 27, 2017 3:59 pm

Disregard last post. I figured it out. Thank you
RobH063
Vectric Apprentice
 
Posts: 83
Joined: Sun Jan 17, 2016 4:19 pm
Location: Jamestown, New York
Model of CNC Machine: 1000mm Xcarve

Re: Help with Pockets Please

Postby Leo » Fri Oct 27, 2017 5:06 pm

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

www.leosworkshop.com
User avatar
Leo
Vectric Wizard
 
Posts: 2418
Joined: Sat Jul 14, 2007 3:02 am
Location: East Freetown, Ma.
Model of CNC Machine: 1300 x 1300 x 254

Re: Help with Pockets Please

Postby martin54 » Fri Oct 27, 2017 5:45 pm

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:
User avatar
martin54
Vectric Wizard
 
Posts: 3277
Joined: Fri Nov 09, 2012 2:12 pm
Location: Crossgates, Scotland
Model of CNC Machine: Gerber System 48 (modified)

Re: Help with Pockets Please

Postby 4DThinker » Sat Oct 28, 2017 2:03 pm

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.
4DThinker
Vectric Wizard
 
Posts: 983
Joined: Sun Sep 23, 2012 12:14 pm
Model of CNC Machine: CNC Shark Pro

Re: Help with Pockets Please

Postby mtylerfl » Sat Oct 28, 2017 2:22 pm

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

carvebuddy.com

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC
User avatar
mtylerfl
Vectric Wizard
 
Posts: 2446
Joined: Thu Jan 29, 2009 3:54 am
Location: Brunswick, GA
Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha

Re: Help with Pockets Please

Postby RobH063 » Sat Oct 28, 2017 2:26 pm

4DThinker, if using the Raster option, would you eliminate the pocket allowance because there would be no need to do a finish pass?
RobH063
Vectric Apprentice
 
Posts: 83
Joined: Sun Jan 17, 2016 4:19 pm
Location: Jamestown, New York
Model of CNC Machine: 1000mm Xcarve

Re: Help with Pockets Please

Postby 4DThinker » Sat Oct 28, 2017 2:36 pm

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
4DThinker
Vectric Wizard
 
Posts: 983
Joined: Sun Sep 23, 2012 12:14 pm
Model of CNC Machine: CNC Shark Pro

Re: Help with Pockets Please

Postby RobH063 » Sat Oct 28, 2017 2:38 pm

Ok, Thank you. I'll give it a try
RobH063
Vectric Apprentice
 
Posts: 83
Joined: Sun Jan 17, 2016 4:19 pm
Location: Jamestown, New York
Model of CNC Machine: 1000mm Xcarve

Re: Help with Pockets Please

Postby Adrian » Sat Oct 28, 2017 3:04 pm

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.
User avatar
Adrian
Vectric Archimage
 
Posts: 7422
Joined: Thu Nov 23, 2006 2:19 pm
Location: Surrey, UK
Model of CNC Machine: ShopBot PRS Alpha 96x48

Re: Help with Pockets Please

Postby RobH063 » Sat Oct 28, 2017 3:13 pm

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.
RobH063
Vectric Apprentice
 
Posts: 83
Joined: Sun Jan 17, 2016 4:19 pm
Location: Jamestown, New York
Model of CNC Machine: 1000mm Xcarve


Return to VCarve - General

Who is online

Users browsing this forum: Timvmax and 21 guests