CAMheads CNC Router Forum By: CAMaster CNC

Go Back   CAMheads CNC Router Forum By: CAMaster CNC > Software > General Discussion

Reply
 
Thread Tools Display Modes
  #1  
Old 06-18-2018, 09:26 AM
kjoiner kjoiner is offline
CAMaster Owner
 
Join Date: Sep 2016
Location: Work - Duluth, GA, Home - Roswell, GA
Posts: 105
Default Chamfers and countersinks - setting size

Hello,

When countersinking using a V bit, or countersink bit, does Vectric have a setting that can determine the depth of cut to achieve the desired diameter or is it just a matter of doing a little trig?

Thanks,

Kyle
__________________
Kyle Joiner
IPA LLC
www.thinkipa.com
Duluth, GA
CAMaster Stinger 1 23
FTC, Laser Cross Hair
Vectric V Carve Pro
Remote Handheld Keypad
Solid Edge ST10
Reply With Quote
  #2  
Old 06-18-2018, 10:02 AM
TinKnocker TinKnocker is offline
CAMaster owner
 
Join Date: Jun 2014
Location: MD
Posts: 298
Default

My daytime job was working in a metal shop, which used a router as one of the metal cutting methods. We found that countersinking with the router did not give the .005 tolerances we required for our stuff. The problem is that a small increase/decrease in depth has a much larger affect on the hypotenuse. We end up using the drill press with a micro-stop to get the correct countersink depths. I wonder if combining the router with the micro-stop might work, but I would worry about the pressure it could apply to the Z-axis.
__________________
-PETE MALONE

SR-34
V-Carve Pro V8
1.7kw Spindle, FTC and counter balance and T-rails
Recoil Ready
Reply With Quote
  #3  
Old 06-18-2018, 11:43 AM
Brian O Brian O is offline
CAMhead Legend
 
Join Date: Oct 2011
Location: Sykesvile Md
Posts: 519
Default

I don't know trig but here's my method. I draw two parallel lines setting the intended depth with two angled lines for the countersink in this case and then measure or adjust.
Attached Files
File Type: crv countersink sample.crv (79.5 KB, 32 views)
__________________
Brian O

stinger III x3

vcarve pro
Reply With Quote
  #4  
Old 06-18-2018, 12:01 PM
BradyWatson BradyWatson is offline
CAMhead Legend
 
Join Date: Oct 2014
Location: 1 hour South of Philly
Posts: 320
Default

Quote:
Originally Posted by kjoiner View Post
is it just a matter of doing a little trig?
Pretty much. I thought the chamfer toolpath would work, but I can't get it to cooperate. (Works in v8.5, but you must use a square end mill...So, nope.)

Attached graphic should get you going.

-B
Attached Images
File Type: jpg CountersinkFormulas.jpg (29.1 KB, 104 views)
__________________
IBILD Solutions - High Definition 3D Laser Scanning Services - Advanced CNC Training and Consultation - Vectric Custom Video Training IBILD.com
Reply With Quote
  #5  
Old 06-18-2018, 12:42 PM
Jim Becker Jim Becker is offline
CAMaster Owner
 
Join Date: Jan 2018
Location: SE PA
Posts: 1,112
Default

Ooh...thanks for that Brady!
__________________
---
Jim Becker

SR-44 (2018), 1.7kw spindle, Performance Premium, USB, Keypad, T-Slot table (y-axis configuration), WinCNC, VCarve Pro upgraded to Aspire

Non CNC stuff...

SCM/Minimax - slider/JP/BS
Festool "a good collection"
Stubby - lathe
Oneida Cyclone
more...

Retired from full time work in the telecom industry 9/2017
Commission work for equestrian tack storage and other custom furniture and cabinetry
Located Bucks County PA
http://bvww.us
bvww.etsy.com
Reply With Quote
  #6  
Old 06-19-2018, 03:37 PM
kjoiner kjoiner is offline
CAMaster Owner
 
Join Date: Sep 2016
Location: Work - Duluth, GA, Home - Roswell, GA
Posts: 105
Default

Thanks for all the replies. I'll just calculate the necessary depth for the cutter. Now that I have the FTC activated on my machine, I'm starting to think about other processes and possible tool changes.

Kyle
__________________
Kyle Joiner
IPA LLC
www.thinkipa.com
Duluth, GA
CAMaster Stinger 1 23
FTC, Laser Cross Hair
Vectric V Carve Pro
Remote Handheld Keypad
Solid Edge ST10
Reply With Quote
  #7  
Old 06-26-2018, 06:26 AM
BrianM BrianM is offline
CAMhead Friend
 
Join Date: Apr 2012
Location: Alcester, U.K
Posts: 5
Default

Quote:
Originally Posted by kjoiner View Post
Hello,

When countersinking using a V bit, or countersink bit, does Vectric have a setting that can determine the depth of cut to achieve the desired diameter or is it just a matter of doing a little trig?

Thanks,

Kyle
The VCarve toolpath will calculate the correct depth based on the diameter of your selected circles and the angle of your tool as long as you can 'drill' the whole depth in one pass.

If the depth of the countersink exceeds the pass depth set for the tool, the VCarve toothpath will make an extra circular pass which your are unlikely to want.


Brian
Reply With Quote
  #8  
Old 06-26-2018, 08:12 AM
kjoiner kjoiner is offline
CAMaster Owner
 
Join Date: Sep 2016
Location: Work - Duluth, GA, Home - Roswell, GA
Posts: 105
Default

Hi Brian,

Thanks for the tip. I'll create a test toolpath and try it out. :)

Kyle
__________________
Kyle Joiner
IPA LLC
www.thinkipa.com
Duluth, GA
CAMaster Stinger 1 23
FTC, Laser Cross Hair
Vectric V Carve Pro
Remote Handheld Keypad
Solid Edge ST10
Reply With Quote
  #9  
Old 06-27-2018, 10:43 AM
JohnnyCNC's Avatar
JohnnyCNC JohnnyCNC is offline
Camaster Owner
 
Join Date: Mar 2009
Posts: 1,148
Send a message via Skype™ to JohnnyCNC
Default

If your V-Bit is the correct angle and is large enough to cut the diameter of the countersink in one pass (i.e. - 1/2" diameter hole and 1" diameter tool) you can take half the diameter of the hole and divide it by the tangent of half the angle of the v-bit (60 v-bit, use 30 for the angle... 90 bit, use 45) to get the depth to plunge.


Those tangent numbers would be approximately 0.5774 for the 60 bit and 1 for the 90 bit.


So if we had a 1/2" diameter hole, we'd do 0.25/0.5774=~0.433" depth for the 60 bit and 0.25/1=0.25" depth for the 90 bit.

You can even plug these numbers into the Drilling Toolpath dialog and let it calculate depth for you.
__________________
JohnnyCNC
Reply With Quote
  #10  
Old 07-23-2018, 03:18 PM
kjoiner kjoiner is offline
CAMaster Owner
 
Join Date: Sep 2016
Location: Work - Duluth, GA, Home - Roswell, GA
Posts: 105
Default

Hello,

I finally tried out the countersink and it worked well. Beats having to set up a drill press or mill to cut the correct depth.

By the way, I found a countersink that works well on plastics - in my case UHMW but I'll also be using it for other plastics as well - maybe even aluminum.

It's McMaster Carr p/n 2742A22. It has reasonable sharp flutes and cuts clean countersinks. I used the drill toolpath and cut down .287 to get a .500 countersink.

Kyle
__________________
Kyle Joiner
IPA LLC
www.thinkipa.com
Duluth, GA
CAMaster Stinger 1 23
FTC, Laser Cross Hair
Vectric V Carve Pro
Remote Handheld Keypad
Solid Edge ST10
Reply With Quote
Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off

Forum Jump


All times are GMT -4. The time now is 12:54 PM.


Powered by vBulletin® Version 3.8.4
Copyright ©2000 - 2019, Jelsoft Enterprises Ltd.