using a different dia bit

This forum is for general discussion regarding VCarve Pro
cusoak
Vectric Wizard
Posts: 486
Joined: Mon Nov 06, 2017 1:57 pm
Model of CNC Machine: Shapeoko 3D XXL

Re: using a different dia bit

Post by cusoak »

In the left picture is of a 1/8" end mil running in a 1/16" toolpath.
Picture on right is the is a 1/8" end mil running in a 1/8" toolpath.
Attachments
kara web 1.jpg

cusoak
Vectric Wizard
Posts: 486
Joined: Mon Nov 06, 2017 1:57 pm
Model of CNC Machine: Shapeoko 3D XXL

Re: using a different dia bit

Post by cusoak »

Here is the right photo
Attachments
kara web 2.jpg

User avatar
FixitMike
Vectric Wizard
Posts: 2173
Joined: Sun Apr 17, 2011 5:21 am
Model of CNC Machine: Shark Pro Plus (retired)
Location: Burien, WA USA

Re: using a different dia bit

Post by FixitMike »

If you are making a pocket cut, use the "Use Larger Area Clearance Tool" option with a 1/8" bit.

If it is a profile cut, run the 1/8" bit and toolpath first, then run a 1/16" bit and toolpath. to finish. (Two different bits and two different toolpaths.)
Good judgement comes from experience.
Experience comes from bad judgement.

LittleGreyMan
Vectric Wizard
Posts: 1012
Joined: Fri May 15, 2015 1:10 pm
Model of CNC Machine: 3 axis small size machine
Location: France

Re: using a different dia bit

Post by LittleGreyMan »

Jeff,

We won't be sure of the answers we give until you post your file.

As Martin noticed, never trick the software until you really master it, to get some special effects or work around a limitation.

If you use a tool instead of another one, you may get unpredictable results (including breaking bits and spoiling material) and will not be able to check your toolpaths with the preview.

If you mill cannot cut the profile with your smallest tool, change your design as Michael suggested.

You're probably just a few clicks away of what you need and the offset function will probably solve your issue.
Best regards

Didier

W7 - Aspire 8.517

User avatar
Leo
Vectric Wizard
Posts: 4082
Joined: Sat Jul 14, 2007 3:02 am
Model of CNC Machine: 1300 x 1300 x 254 Chinese Made
Location: East Freetown, Ma.
Contact:

Re: using a different dia bit

Post by Leo »

cusoak wrote:In the left picture is of a 1/8" end mil running in a 1/16" toolpath.
Picture on right is the is a 1/8" end mil running in a 1/8" toolpath.
Both of the pictures you posted here are precisely what I would expect to see with the descriptions you described.

On the 1/8 cutter with a 1/16 toolpath.
The end result looks good to me.
BUT it is NOT actually correct.
What the cutter did was to cut away more material that it was supposed to do - see Adrians sketch. The cutter cut 1/32 more material that a 1/16 cutter would have cut. You cheated the software a bit. Nothing wrong with that as long as you get what you want.

On the 1/8 cutter with a 1/8 toolpath
The preview and end result IS what is expected.
In actuality the 1/8 cutter cannot fit into the areas as drawn, so the software calculate toolpath where the cutter CAN fit and does not go where the cutter fit.

In order to use a 1/8 cutter the vector drawing will need to modified so that the cutter can fit all around. Using the solid toolpath preview is a GREAT tool to see where the cutter can fit.
Imagine the Possibilities of a Creative mind, combined with the functionality of CNC

User avatar
highpockets
Vectric Wizard
Posts: 3667
Joined: Tue Jan 06, 2015 4:04 pm
Model of CNC Machine: PDJ Pilot Pro

Re: using a different dia bit

Post by highpockets »

Looking at your pictures, re-read Michael's post, you will not be able to get an 1/8" bit to cut into the same areas of a 1/16" bit, it just won't fit.
John
Maker of Chips

User avatar
martin54
Vectric Archimage
Posts: 7339
Joined: Fri Nov 09, 2012 2:12 pm
Model of CNC Machine: Gerber 48, Triac PC, Isel fixed gantry
Location: Kirkcaldy, Scotland

Re: using a different dia bit

Post by martin54 »

OK having looked at the pictures then I would simply edit the artwork a little as Michael has already said, easy enough to do & only take a couple of minutes (if that), a simple offset may even do the trick, the good thing is that the preview will show you so no wasted material :lol: :lol:

cusoak
Vectric Wizard
Posts: 486
Joined: Mon Nov 06, 2017 1:57 pm
Model of CNC Machine: Shapeoko 3D XXL

Re: using a different dia bit

Post by cusoak »

This was a profile cut on the outside. cutting all the way through.
The words were welded to the top of the board .So the same tool path cut all the way around the plaque to cut it out of a blank.
I not sure which comment is Micheal's
Jeff
This would all be easier if I could find 1/16" end mill that has a 3/4" cutter lenght.
I will post a picture of the finished project.
Jeff

User avatar
martin54
Vectric Archimage
Posts: 7339
Joined: Fri Nov 09, 2012 2:12 pm
Model of CNC Machine: Gerber 48, Triac PC, Isel fixed gantry
Location: Kirkcaldy, Scotland

Re: using a different dia bit

Post by martin54 »

mtylerfl wrote:Hi Jeff,

The 1/8” Bit cannot fit into the same nooks and crannies as a 1/16”.

When designing, I will often draw a circle representing the diameter of the Bit I plan to use. Actually a teeny amount larger than the diameter to be in the safe side.

This circle is a handy reference during the design process. I can move the circle into tight corners or spaces to see if the Bit will fit or not.

If the Bit won’t fit, I will adjust/edit my design until it does fit. Then I will create Toolpaths to view the simulation using that bit diameter to see the actual result.

So, you have a choice. Either enlarge and/or edit your design so the 1/8” Bit will fit into your tight spots, or use your smaller 1/16” bit and use the thinner material suitable for that bit.
This is Michael's post which talks about making sure the tool you have to cut with fits when you are designing :lol: :lol:

User avatar
mtylerfl
Vectric Archimage
Posts: 5865
Joined: Thu Jan 29, 2009 3:54 am
Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha
Location: Brunswick, GA

Re: using a different dia bit

Post by mtylerfl »

Hi Jeff,

I don’t know if an “off the shelf” 1/16” diameter bit that would have a 3/4” depth of cut exists.

Perhaps it does, but if you find it, you might want to purchase several. I anticipate breaking some during the process of dialing in “survivable” pass depths and feed rates!
Michael Tyler

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC

User avatar
highpockets
Vectric Wizard
Posts: 3667
Joined: Tue Jan 06, 2015 4:04 pm
Model of CNC Machine: PDJ Pilot Pro

Re: using a different dia bit

Post by highpockets »

Not to say there isn't one, I just haven't found a 1/6" EM with a 3/4" CL.

You might try a 1.5mm tapered ball nose, I have some that are 3" OAL with a CL of 1 1/4". You'd have to clean up the bottom edge (or set the toolpath cut depth .8mm deeper than the material thickness) and you'd have a very shallow bevel on the cut edge.

Michael beat me to it.... :D
John
Maker of Chips

ger21
Vectric Wizard
Posts: 1592
Joined: Sun Sep 16, 2007 2:59 pm
Model of CNC Machine: Custom DIY
Location: Lake St Clair, MI, USA
Contact:

Re: using a different dia bit

Post by ger21 »

You might try a 1.5mm tapered ball nose, I have some that are 3" OAL with a CL of 1 1/4". You'd have to clean up the bottom edge (or set the toolpath cut depth .8mm deeper than the material thickness) and you'd have a very shallow bevel on the cut edge.
At the surface, where it really matters, it's likely to still be the same size or larger than a 1/8" straight bit.
Gerry - http://www.thecncwoodworker.com

User avatar
Leo
Vectric Wizard
Posts: 4082
Joined: Sat Jul 14, 2007 3:02 am
Model of CNC Machine: 1300 x 1300 x 254 Chinese Made
Location: East Freetown, Ma.
Contact:

Re: using a different dia bit

Post by Leo »

YES the cutter you are looking for DOES exist.

Harvey Tool has a 1/16 cutter that can cut .625 or .720

Harvey is a HIGH quality tool.

http://www.harveytool.com/ToolTechInfo. ... ber=951360 $45.00 each

http://www.harveytool.com/ToolTechInfo. ... mber=34960 $57.00 each

Depending on Spindle rigidity, work holding rigidity, spindle run out, correct feeds and speeds, material stability - cutters of this length to diameter ratio are EXTREMELY EASY to break. I mean as soon as the cutter touches the material they break.

I don't believe a Shapeko has what it takes.

In my estimation I feel you have about a 10% chance or less of success with the harvey tool. I have used these kinds of tools, with success, and I have broken tools as well. Personally for what you are doing I would not use these tools

It MAY seem like the easiest way out ---- BUT

BUT - there is more than one way to skin a cat. Sometimes a compromise is in order

Several very good suggestions have already been made that will ensure success by several posters.

Tapered end mills are VERY strong for the job they do - MUCH stronger than a straight fluted tool that I linked to at Harvey.
Imagine the Possibilities of a Creative mind, combined with the functionality of CNC

Post Reply