Help creating form tool for single flute upcut spiral

This forum is for general discussion about Aspire

Help creating form tool for single flute upcut spiral

Postby bobrickard » Tue Jun 26, 2018 2:26 pm

I'm trying to create a form tool for an Onsrud 63-631 one flute upcut spiral bit. This is the opposite of a V bit in that the "point" is at the edge rather that at the center. This does not seem possible in Aspire. I get an error that a line sloping from the center to the edge is not a suitable vector, whereas sloping from the edge to the center is fine. Am I missing something? I want to be able to use preview mode to see the "islands" left when cutting is confined to a tight space and the bit doesn't move across the center, leaving a high section.
bobrickard
 
Posts: 21
Joined: Fri Jul 05, 2013 9:42 pm
Location: Bloomingdale NJ
Model of CNC Machine: Shopbot Desktop MAX

Re: Help creating form tool for single flute upcut spiral

Postby Adrian » Tue Jun 26, 2018 2:37 pm

You can't create a tool that would lead to any sort of undercut.

http://support.vectric.com/aspire-quest ... h-undercut

As long as you're using a stepover of no more than 40% I wouldn't think that profile would leave any islands.
User avatar
Adrian
Vectric Archimage
 
Posts: 8214
Joined: Thu Nov 23, 2006 2:19 pm
Location: Surrey, UK
Model of CNC Machine: ShopBot PRS Alpha 96x48

Re: Help creating form tool for single flute upcut spiral

Postby ger21 » Tue Jun 26, 2018 3:15 pm

A 63-631 is a 1/2" endmill.
No need to create a form tool.
Gerry
ger21
Vectric Wizard
 
Posts: 1044
Joined: Sun Sep 16, 2007 2:59 pm
Location: Shelby Township, MI, USA

Re: Help creating form tool for single flute upcut spiral

Postby martin54 » Tue Jun 26, 2018 4:50 pm

What is it you are wanting to do with the tool? Can you post a screenshot or something, as ger21 says the bit you have mentioned is a single flute endmill so would normally be entered the same as any other endmill, the fact that it is single flute & designed to cut aluminium is only relevant when it comes to setting the spindle speed, feedrate stepover etc :lol: :lol:
User avatar
martin54
Vectric Wizard
 
Posts: 3786
Joined: Fri Nov 09, 2012 2:12 pm
Location: Crossgates, Scotland
Model of CNC Machine: Gerber System 48 (modified)

Re: Help creating form tool for single flute upcut spiral

Postby bobrickard » Tue Jun 26, 2018 7:36 pm

I'm doing pocket toolpaths with a 0.5" clearance path and a 0.125" finish path. Aspire generates paths just fine, but has to do so without regard to the geometry of the end mill. The preview, however, does show how the tool shape effects the cut. I would like to define a single flute spiral end mill as a form tool just so the preview will be realistic.

For example, if I want to cut this:

1) goal.png


Here is the pocket specification:

2) toolpaths.png


And this is the preview for just the 0.5" clearance pass:

3) preview 0.5 only.png


Which looks great. However, here is the result (just the clearance pass):

4) result 0.5 only.jpg


Note the artifacts in three smallest circles. Running the 0.125" finish path doesn't get rid of these, as Aspire doesn't know they are there. And from the preview, I don't either until I run the job. If I can spot them before I cut, then I can adjust the design to change the dimensions of those problem areas. In this sample, those areas are pretty easy to identify. But as they piece gets larger and more complex, not so much:

5) example.jpg


So how can I create a form tool to represent this:

8) so how this.png


Or what other approach can I take?
bobrickard
 
Posts: 21
Joined: Fri Jul 05, 2013 9:42 pm
Location: Bloomingdale NJ
Model of CNC Machine: Shopbot Desktop MAX

Re: Help creating form tool for single flute upcut spiral

Postby Adrian » Tue Jun 26, 2018 7:42 pm

As I said you can't create a form tool like that. The inner point of the profile cannot be below the outer point. You have to define it as an end-mill and allow for the islands yourself. You can't preview them.
User avatar
Adrian
Vectric Archimage
 
Posts: 8214
Joined: Thu Nov 23, 2006 2:19 pm
Location: Surrey, UK
Model of CNC Machine: ShopBot PRS Alpha 96x48

Re: Help creating form tool for single flute upcut spiral

Postby TReischl » Tue Jun 26, 2018 9:22 pm

Apparently you will get these artifacts anytime the feature is less than 2X the diameter of the bit. So maybe that will help you determine when it is going to happen, before it happens.
http://www.tedreischl.com

Low Profile CNC Router Vise
User avatar
TReischl
Vectric Wizard
 
Posts: 2064
Joined: Thu Jan 18, 2007 6:04 pm
Location: Leland NC
Model of CNC Machine: 8020 Build 48X36X8 RP 2010 Screenset

Re: Help creating form tool for single flute upcut spiral

Postby bobrickard » Tue Jun 26, 2018 9:48 pm

Sorry, Adrian. I misunderstood your comment. I interpreted "undercut" to mean a cutting edge on a top surface of the end mill, like a t-slot bit or this one:

Screen Shot 2018-06-26 at 4.41.24 PM.png


As much as I like the Onsrud single flute spiral, I may need to switch to something else that clears fully when the area is less than 2X the bit diameter.
bobrickard
 
Posts: 21
Joined: Fri Jul 05, 2013 9:42 pm
Location: Bloomingdale NJ
Model of CNC Machine: Shopbot Desktop MAX

Re: Help creating form tool for single flute upcut spiral

Postby mtylerfl » Wed Jun 27, 2018 2:27 am

Perhaps simply switch to a "flat-end" Upcut End Mill and your troubles are over. :D

I have a Whiteside Spiral Upcut 2-flute 1/2" EM Part# RU5100 that would likely work for what you are doing. Many other brands that would work fine as well.
Michael Tyler

carvebuddy.com

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC
User avatar
mtylerfl
Vectric Wizard
 
Posts: 3005
Joined: Thu Jan 29, 2009 3:54 am
Location: Brunswick, GA
Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha

Re: Help creating form tool for single flute upcut spiral

Postby Mobius » Fri Jun 29, 2018 5:15 am

mtylerfl wrote:Perhaps simply switch to a "flat-end" Upcut End Mill and your troubles are over. :D

I have a Whiteside Spiral Upcut 2-flute 1/2" EM Part# RU5100 that would likely work for what you are doing. Many other brands that would work fine as well.


This. If your pocket is less than double the size of the bit you are using, you need to use a flat bottom end mill to get a result like the simulation. It wouldn't matter if you could draw the bit the way you are asking, the result would be the same.
Connor Bredin
Distinctive Dimensional Concepts Ltd.
www.distinctive-concepts.ca
Mobius
Vectric Wizard
 
Posts: 320
Joined: Wed Jul 09, 2014 1:19 am
Location: Drumheller, Alberta, Canada
Model of CNC Machine: CRP Pro 4848 Custom Build


Return to Aspire - General

Who is online

Users browsing this forum: Google [Bot], SuperDave and 23 guests