How to Pocket using Offset from outside inward ?

This section is for useful tips and tricks for Aspire
Post Reply
Darryl Kerney
Posts: 18
Joined: Sun Oct 18, 2020 10:24 pm
Model of CNC Machine: Ultimatik Mini

How to Pocket using Offset from outside inward ?

Post by Darryl Kerney »

Maybe there is a reason not to do it but it seems to me it would work for what i want to do, which is use Pocket to level material with a 1/2" end mill using the offset function so that it uses Climb milling the entire time and works it's way from the OUTSIDE to the middle. But it always ends up starting in the middle and going outward. i do not want to use raster since it alternates between Climb and Conventional as it goes back and forth, but if i do so is it better to go with the wood grain or across it ?
IS there a good reason why it wouldn't be good to go from outside in with Climb for every pass ?
Also, i tried using boxes i drew and then vector selection order from outside in, with Profile, set to Climb, but it alternates back and forth between Climb and Conventional too instead of doing Climb for every pass !
What the heck ?

User avatar
TReischl
Vectric Wizard
Posts: 4079
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset
Location: Leland NC

Re: How to Pocket using Offset from outside inward ?

Post by TReischl »

Nope, in all my years I have not figured out a way to do what you suggest. Climb cutting from the outside in is a good technique in that it prevents chipouts on the edge of the part.

As to rastering with or across the grain? Sort of a mixed bag. I had done both and all sorts of angles. Going with the grain and taking a nice healthy cut, like 50% diameter often causes nasty stringy chips on the conventional pass that clog up the dust collector. I tend to use a 45 degree angle to prevent that.

I suppose a person could take a light profile pass around the outside of a piece using climb and then just pocket out the rest.
"If you see a good fight, get in it." Dr. Vernon Jones

Darryl Kerney
Posts: 18
Joined: Sun Oct 18, 2020 10:24 pm
Model of CNC Machine: Ultimatik Mini

Re: How to Pocket using Offset from outside inward ?

Post by Darryl Kerney »

Thanks. It sure is strange there isn't a way to do that, I thought my idea of using ever smaller boxes from the outside going inward and using Profile with Vector Selection order was going to work, then it went and alternated between Climb and Conventional, maybe the way is to do each pass as a single toolpath and then merge them all ? Sure seems like a lot of extra time to do something seemingly simple though. I will try it and see if it works.

Darryl Kerney
Posts: 18
Joined: Sun Oct 18, 2020 10:24 pm
Model of CNC Machine: Ultimatik Mini

Re: How to Pocket using Offset from outside inward ?

Post by Darryl Kerney »

OK i tried something that seems to work,
i started with a 4x4" project to keep it small to save time in preview Sim,
i drew a box around the outside, so 4x4,
then half inch smaller each time, with 1/2" end mill as the bit,
then did Profile cut ON the vector for each them using Climb,
so it's individual Profile cuts for each box that i drew that are 1/2 inch smaller going inwards,
then i merged them with the only option selected being Merge By Part,
it works !
it goes from outside in using Climb cut the whole time, without lifting either, so like a pocket cut where it moves inward instead of outward.
each cut overlaps the previous one by 50% so it should leave a nice finish,
especially since i plan to get the Amana 51637-K "Low Helix Finisher" bit,
which i cannot find in the Tool Database, i guess it is newer than the what they have in the database download...

dfwexhibit
Posts: 14
Joined: Sat Nov 17, 2018 6:11 pm
Model of CNC Machine: AXYZ 5010
Location: Fort Worth, TX
Contact:

Re: How to Pocket using Offset from outside inward ?

Post by dfwexhibit »

To prevent tear-out when I cut pockets in solid wood, I cut a full tool width profile path inside the shape then follow it up with a second pocket path with an allowance set so that it doesn't touch the edges of my first profile cut. I never get any kind of "tear-up" within the pocket at the bottom of the cut, so I don't care which direction it pockets-out the bulk of the material. I just don't want a partial width cut along the perimeter because regardless of the climb or conventional direction, it will always have potential for tear out on one or more edges.

It baffles me why the developer doesn't simply add the option to flip inside-out to outside-in for offset pockets. Keep the same climb and conventional options because they're still useful when you pocket either direction, depending on the species of wood you cut.

Also, Vectric, please show the damned start point when drawing the pocket preview... I want to see the plunge point because your pocket toolpaths are horrible and you often make numerous lifts and plunges in pockets where they are not needed. Plus, you have a bug that plunges the bit straight down sometimes without ramping even with ramping set, and that's an absolute NO-NO with compression and down-flute bits. Will post this bug in another thread too.
----------------------------------------
klevr.us, dfwexhibit.com, bergdesign.com

Post Reply