using a different dia bit
-
- 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
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.
Picture on right is the is a 1/8" end mil running in a 1/8" toolpath.
- FixitMike
- Vectric Wizard
- Posts: 2177
- 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
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.)
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.
Experience comes from bad judgement.
-
- Vectric Wizard
- Posts: 1013
- 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
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.
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
Didier
W7 - Aspire 8.517
- Leo
- Vectric Wizard
- Posts: 4092
- 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
Both of the pictures you posted here are precisely what I would expect to see with the descriptions you described.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.
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
- 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
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
Maker of Chips
- martin54
- Vectric Archimage
- Posts: 7355
- 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
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
-
- 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
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
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
- martin54
- Vectric Archimage
- Posts: 7355
- 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
This is Michael's post which talks about making sure the tool you have to cut with fits when you are designingmtylerfl 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.
- mtylerfl
- Vectric Archimage
- Posts: 5896
- 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
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!
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
facebook.com/carvebuddy
-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC
- 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
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....
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....
John
Maker of Chips
Maker of Chips
-
- 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
At the surface, where it really matters, it's likely to still be the same size or larger than a 1/8" straight bit.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.
Gerry - http://www.thecncwoodworker.com
- Leo
- Vectric Wizard
- Posts: 4092
- 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
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.
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