Official Luthiers Forum!

Owned and operated by Lance Kragenbrink
It is currently Thu Mar 28, 2024 7:07 pm


All times are UTC - 5 hours





Post new topic Reply to topic  [ 15 posts ] 
Author Message
PostPosted: Wed Jun 05, 2013 1:46 am 
Offline
Mahogany
Mahogany

Joined: Tue Oct 14, 2008 9:38 pm
Posts: 79
Location: Peters Creek,Alaska
Wondering if anyone has a CAM program that will link profile cuts and the ability to remove the entry/exit moves between linked curves so that feed speeds can be changed while retaining movement continuity. I have BC and RhinoCAM and haven't been able to figure out how to to it. I have gone in to the code and manually changed the speeds but it seems like there should be a way to do this. I am trying to slow things down on corner neck/headstock cuts to avoid blowout.
Thanks,
Mike
Image


Top
 Profile  
 
PostPosted: Wed Jun 05, 2013 8:49 am 
Offline
Contributing Member
Contributing Member

Joined: Mon Jan 28, 2013 8:29 pm
Posts: 113
First name: Rand
Last Name: Kennedy
State: CO
Focus: Build
Status: Semi-pro
My controller has acceleration control features that slow it down for corners. Not sure what you are using but perhaps take a look in the controller.

Interesting toolpath with the loopies, not sure I like that. I only profile the headstock sides and the tenon/heel area, the important vertical stuff, and let surfacing take care of the rest. Certainly not going for speed. YMMV


Top
 Profile  
 
PostPosted: Wed Jun 05, 2013 10:02 am 
Offline
Contributing Member
Contributing Member
User avatar

Joined: Thu Jun 12, 2008 6:59 am
Posts: 1963
Location: Rochester Michigan
Slowing down at the corners won't necessarily prevent blowouts. What I do which has served me well is to do exactly what you'd do if you were using hand tools - Climb cut any end grain features first and then go back and climb cut long grain. In the end it will add a bit of time but you can pretty much eliminate any chance of blowout this way.

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com


Top
 Profile  
 
PostPosted: Wed Jun 05, 2013 10:18 am 
Offline
Mahogany
Mahogany

Joined: Tue Oct 14, 2008 9:38 pm
Posts: 79
Location: Peters Creek,Alaska
Thanks for the information, I am climb cutting but not addressing the end grain first, I will try that. I am using Mach maybe a CV setting would slow things on any moves greater or less a certain angle, will look.


Top
 Profile  
 
PostPosted: Wed Jun 05, 2013 12:58 pm 
Offline
Contributing Member
Contributing Member

Joined: Mon Jan 28, 2013 8:29 pm
Posts: 113
First name: Rand
Last Name: Kennedy
State: CO
Focus: Build
Status: Semi-pro
Where are you having the tearout ? As Andy says splitting it up into separate ops is good. My headstock end is G style, perpendicular to the face, so it can't be final cut via profile. I use a z-level (waterline, horizontal - whatever yours is called) finish surfacing strategy to finally pick that up, last of 7 ops to slowly whittle it down.


Top
 Profile  
 
PostPosted: Wed Jun 05, 2013 2:44 pm 
Offline
Mahogany
Mahogany

Joined: Tue Oct 14, 2008 9:38 pm
Posts: 79
Location: Peters Creek,Alaska
I have struggled for the most part at the end of the headstock. I have worked it out with slow successive light climb passes around the headstock working my way in, but wanted to figure out a different way on a new neck shape. Wondering what style flute you all may be using for this portion of your work. I have been using a ball end spiral up-cut but wondering about straight and down cut and also flat vs. round. Thanks again for the information.

Image


Top
 Profile  
 
PostPosted: Wed Jun 05, 2013 3:47 pm 
Offline
Brazilian Rosewood
Brazilian Rosewood
User avatar

Joined: Tue May 02, 2006 9:02 am
Posts: 2351
Location: Canada
First name: Bob
Last Name: Garrish
City: Toronto
State: Ontario
Country: Canada
Status: Professional
What Andy said is good advice, I used that exact approach for avoiding chipping on ebony fretboards in product and also use it on things like headstocks with points.

If you're having substantial top-edge blowout then you can mitigate it by using a ball and doing a few passes successively rolling over the edge. It's a good way to keep sharp corners, and it avoids having to use other options like down-spiral cutters which necessitate more tool changes and stocking more tools. On the plus side, it takes forever and a day to wear out a carbide tool if you're only cutting wood, so it's not like you'll ever have to replace them unless you're running a production shop.

I never used any tools except standard carbide endmills on production on necks until I was using custom insert cutters. I can see how a left hand spiral cutter could help on some operations if you have a tool changer. There was always something else that could be done to mitigate problems without using special tooling.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services


Top
 Profile  
 
PostPosted: Wed Jun 05, 2013 3:57 pm 
Offline
Contributing Member
Contributing Member

Joined: Mon Jan 28, 2013 8:29 pm
Posts: 113
First name: Rand
Last Name: Kennedy
State: CO
Focus: Build
Status: Semi-pro
One of my necks is similar to yours except for the headstock shape and tenon. It looks like your headstock end is the same angle as your headstock so you are profiling this ? Like a PRS, not like a G ? I like Andy's suggestion of climb cutting across that while you still have some extra stock on the sides for support, before profiling the sides.

My order of operations on the face down is:
1 Planar rough (.5" roughing end mill) set it aside to do the wild thing. True up or toss if excessive
2 Profile the sides of the headstock. Rough then finish cut. (.5" BM uses the sides not the end of the bit)
3 Planar finish the horizontal surface features (.5" BM)
4 Planar finish the more vertical areas of the neck shaft with smaller stepover (.5" BM)
5 Planar finish the headstock blend area smaller stepover different angle of attack (.5" BM)
6 Z-Level finish the headstock end (.25" BM due to minimum radius)

Again my headstock end is perpendicular to the headstock face. I do it last because of the tool change. I used to do what I could with the .5 BM but with the z-finish, tearout wasn't a problem so I eliminated that.


Top
 Profile  
 
PostPosted: Wed Jun 05, 2013 4:19 pm 
Offline
Contributing Member
Contributing Member

Joined: Thu Mar 19, 2009 10:16 pm
Posts: 189
Location: Bell Buckle, TN.
First name: kevin
Last Name: waldron
City: Bell Buckle
State: TN
Zip/Postal Code: 37020
Country: USA
Focus: Build
Status: Professional
Your work looks good!

We approach the toolpathing a lot different. We use regions for defining the various operations. We typically will draw the regions below the part as shown in our attachments and usually set this for 1/2 of the ball nose that we use. Most times we only use 2 to 3 tools total. We have a large cnc and it is capable of cutting at 1200 IPM but for small parts we usually set it with the ball nose for 600 ipm...... the idea is that it can't accelerate or decelerate anywhere close to these speeds in short distances but we let the machine work all this out. This neck shown usually takes about 30 minutes from start to finish once setup..... but note the time that the software says.

Hope this helps need more information contact us off-site. www.waldronmusic.com

Blessings,

Kevin


You do not have the required permissions to view the files attached to this post.


Top
 Profile  
 
PostPosted: Wed Jun 05, 2013 8:21 pm 
Offline
Contributing Member
Contributing Member
User avatar

Joined: Thu Jun 12, 2008 6:59 am
Posts: 1963
Location: Rochester Michigan
Fleck wrote:
I am using Mach maybe a CV setting would slow things on any moves greater or less a certain angle, will look.


There is a setting in Mach 3 on the general config page - something like stop CV on angles > "X" or something like that. I believe I have mine set at 80˚. This will cause the machine to switch to exact stop on a trajectory change in angle of 80˚ or more. i.e., if you set it for 45˚ the angle cut in the part is 135˚.

This also keeps it from rounding corners if your machine has high feedrates but only so so acceleration (like mine does). I can cut at 400ipm but my accel on my X is only 35

But, this still won't solve your problem. Cutting the end grain first will.

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com


Top
 Profile  
 
PostPosted: Wed Jun 05, 2013 8:32 pm 
Offline
Koa
Koa
User avatar

Joined: Sat Jan 08, 2005 4:19 am
Posts: 1534
Location: United States
First name: Nelson
Last Name: Palen
One method of eliminating tearout at the end of a cut is to drill a hole at that location prior to milling the contour. For example, when cutting fretboards, I use the same 1/4" endmill to plunge a hole at the two opposite corners of the fretboard prior to milling the perimeter with the same tool.


Top
 Profile  
 
PostPosted: Wed Jun 05, 2013 11:01 pm 
Offline
Cocobolo
Cocobolo

Joined: Mon Mar 03, 2008 6:51 pm
Posts: 488
I tried a 1/4" compression spiral on headstock end grain recently. The assumption being that a smaller diameter cutter would spend less time cutting perpendicular to the grain. I used 2 or 3 full depth passes with a stopover of .25 mm. It worked pretty well.


Top
 Profile  
 
PostPosted: Thu Jun 06, 2013 10:28 am 
Offline
Mahogany
Mahogany

Joined: Tue Oct 14, 2008 9:38 pm
Posts: 79
Location: Peters Creek,Alaska
Thanks for all the information.


Top
 Profile  
 
PostPosted: Thu Jun 06, 2013 6:02 pm 
Offline
Brazilian Rosewood
Brazilian Rosewood
User avatar

Joined: Tue May 02, 2006 9:02 am
Posts: 2351
Location: Canada
First name: Bob
Last Name: Garrish
City: Toronto
State: Ontario
Country: Canada
Status: Professional
Sheldon Dingwall wrote:
I tried a 1/4" compression spiral on headstock end grain recently. The assumption being that a smaller diameter cutter would spend less time cutting perpendicular to the grain. I used 2 or 3 full depth passes with a stopover of .25 mm. It worked pretty well.


I always suspected the compression cutters might make a mess in the middle, but nice to hear they do an alright job. Totally true about the smaller cutters; you can get a smoother cut overall with larger cutters due to the edge speed but smaller cutters are way less likely to chip out. Before I started ordering my cuts strategically, I used a 1/8" cutter for everything dangerous.

Kevin Waldron wrote:
... the idea is that it can't accelerate or decelerate anywhere close to these speeds in short distances but we let the machine work all this out. This neck shown usually takes about 30 minutes from start to finish once setup..... but note the time that the software says.


Ain't that the truth! I wasn't expecting such a big difference since it look liked your machine had really high accel for a router in the video I saw. The Fadal (AFTER retrofit) was running a 14 minute program in 15-16 minutes with a programmed feed of 400 IPM, but the pre-retrofit acceleration was less than a third what it was running post-retro. My new machine, a mid-90s industrial router (6000lbs), has a max feed of 300 IPM but the motors are specced so close that it takes the thing a 8-12 inches of run-up to hit that speed! It took 6 hours to run a reported 50 minute program at 120IPM because it was all small features! Can't wait to get some free time to put the linear motors on and see what terrifyingly fast looks like, it's been quite awhile since I've seen regular fast!

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services


Top
 Profile  
 
PostPosted: Thu Jun 06, 2013 10:01 pm 
Offline
Contributing Member
Contributing Member

Joined: Thu Mar 19, 2009 10:16 pm
Posts: 189
Location: Bell Buckle, TN.
First name: kevin
Last Name: waldron
City: Bell Buckle
State: TN
Zip/Postal Code: 37020
Country: USA
Focus: Build
Status: Professional
Bob,

We can crank up the accerleration about 3 time faster but cuts/tearouts, tearing the neck off the fixture, and sanding increase ........... easier to let the machine do the work than us sand it manually or have to compensate for extra material especially when we are cutting the 4" tall guitar heels. One problem on the tall hills is breaking the vacuum when the heel height increases and the speed is increased ...... probably double the speed on a low profile neck.... we haven't cut to many electric necks....we've tried to stay out of this market..... to competitive for our liking. (Our machine weighs over 10,000 lbs..... so it takes a lot to move, stop, and start things rolling)

Blessings,

Kevin


Top
 Profile  
 
Display posts from previous:  Sort by  
Post new topic Reply to topic  [ 15 posts ] 

All times are UTC - 5 hours


Who is online

Users browsing this forum: No registered users and 15 guests


You cannot post new topics in this forum
You cannot reply to topics in this forum
You cannot edit your posts in this forum
You cannot delete your posts in this forum
You cannot post attachments in this forum

Jump to:  
Powered by phpBB® Forum Software © phpBB Group
phpBB customization services by 2by2host.com