Need quick explaination of step over

This forum is for general discussion regarding VCarve Pro

Need quick explaination of step over

Postby SIBUD » Sun Mar 03, 2013 3:34 pm

What is it? When and why do I use it?

Thanks in advance.

PS I looked in the documentation and couldn't find an explanation other than how to set it.
Bud Meade
Nashville, IL

"Without deadlines, nothing would be done."
User avatar
SIBUD
Vectric Craftsman
 
Posts: 193
Joined: Sun Jan 06, 2013 8:32 pm
Location: Nashville, IL
Model of CNC Machine: Signal Seeker 24X24

Re: Need quick explaination of step over

Postby zeeway » Sun Mar 03, 2013 3:38 pm

When doing 3D carving or pocket machining, your tool cuts the next pass offset sideways at a percentage of the diameter. For example on a .125 inch tool, at 9% stepover, the next pass moves over (9% x .125=) .01125 inches. So a one inch wide piece would require (1 /.01125=) 89 passes. The less the stepover, the finer the detail. From 8 to 10% is a good value for finish passes on 3D work. For rough passes, you could use 40 to 60%. Pocket machining with an end mill, I would use 30 to 40% stepover.

Angie
User avatar
zeeway
Vectric Wizard
 
Posts: 2755
Joined: Thu Feb 11, 2010 9:24 pm
Location: SC, USA
Model of CNC Machine: Joe's Hybrid CNC with Cast CNC top end

Re: Need quick explaination of step over

Postby Leo » Sun Mar 03, 2013 4:20 pm

Angie nailed it on the 3D stuff.

On 3D - with a ball nosed tool - I will step over at 5% or so. Depending on the tool and the profile, I like to see .005 to .010.

If I was just doing a flat bottom pocket I would stepover at about 90%.

Figure this ---- The tool can cut a slot. That is 100%. Well with that in mind I want the best efficiency in time - so if the tool is capable of 100%, then with a small overlap in passes at 90% - that will be fine.
Imagine the Possibilities of a Creative mind

http://www.mishacustom.com
User avatar
Leo
Vectric Wizard
 
Posts: 1120
Joined: Sat Jul 14, 2007 3:02 am
Location: East Freetown, Ma.
Model of CNC Machine: Modified - Larken Camtool 2424 / Mach3

Re: Need quick explaination of step over

Postby SIBUD » Sun Mar 03, 2013 4:36 pm

Thanks to you both. I think I understand it.

When using a V bit to carve letters, is step over an issue or should it be set to 0?
Bud Meade
Nashville, IL

"Without deadlines, nothing would be done."
User avatar
SIBUD
Vectric Craftsman
 
Posts: 193
Joined: Sun Jan 06, 2013 8:32 pm
Location: Nashville, IL
Model of CNC Machine: Signal Seeker 24X24

Re: Need quick explaination of step over

Postby Leo » Sun Mar 03, 2013 4:55 pm

SIBUD wrote:Thanks to you both. I think I understand it.

When using a V bit to carve letters, is step over an issue or should it be set to 0?


zero step over on v-grooving - BUT

If you have a flat depth set - then yes there will be a step over amount. It will be small because you will be doing the step over based on the tip of the tool.

Step over is a sideways motion
Imagine the Possibilities of a Creative mind

http://www.mishacustom.com
User avatar
Leo
Vectric Wizard
 
Posts: 1120
Joined: Sat Jul 14, 2007 3:02 am
Location: East Freetown, Ma.
Model of CNC Machine: Modified - Larken Camtool 2424 / Mach3

Re: Need quick explaination of step over

Postby tmerrill » Sun Mar 03, 2013 4:57 pm

Hi Bud,

See if this helps:

If the v-carve is going to be cut with a single pass, then the Stepover values are not used.

If the v-carve is too deep and wide to be cut in a single pass, the depth for each pass is controlled by the Pass Depth you have set for the v-bit and the "Clearance Pass Stepover" controls how much horizontal movement takes place as the v-bit 'clears' the center material for that pass. This can be as coarse as your machine/bit/setup allows as it is just roughing out material which will all be removed when the toolpath completes.

If you have the Flat Depth option checked, the "Final Pass Stepover" controls how 'smooth' the flat bottom will be. The smaller the stepover, the smoother it will be however with a true v-bit (comes to a point) you will always see ridges. Also, the smaller the stepover, the longer the machining time. If you are using the Flat Depth option, it is always best to use an endmill to clear the flat areas and then the v-bit will only need to clear any flat areas where the endmill could not reach.

You can easily see the effects of different settings by calculating the toolpath, preview it and inspect the blue lines. These lines are where the very point of the v-bit will be traveling.

Tim
tmerrill
Vectric Archimage
 
Posts: 4794
Joined: Thu May 18, 2006 3:24 pm
Location: North Carolina
Model of CNC Machine: ShopBot

Re: Need quick explaination of step over

Postby SIBUD » Sun Mar 03, 2013 5:08 pm

Thanks Leo and Tim.

Your explanations make it perfectly clear.

I'm like a sponge, soaking up a lots of information.
Bud Meade
Nashville, IL

"Without deadlines, nothing would be done."
User avatar
SIBUD
Vectric Craftsman
 
Posts: 193
Joined: Sun Jan 06, 2013 8:32 pm
Location: Nashville, IL
Model of CNC Machine: Signal Seeker 24X24

Re: Need quick explaination of step over

Postby Leo » Sun Mar 03, 2013 8:22 pm

Nothing wrong with sponges - I are one too. :D
Imagine the Possibilities of a Creative mind

http://www.mishacustom.com
User avatar
Leo
Vectric Wizard
 
Posts: 1120
Joined: Sat Jul 14, 2007 3:02 am
Location: East Freetown, Ma.
Model of CNC Machine: Modified - Larken Camtool 2424 / Mach3


Return to VCarve Pro - General

Who is online

Users browsing this forum: Google [Bot] and 6 guests