45 Degree slice.

This forum is for general discussion regarding VCarve Pro
Post Reply
W2csa
Posts: 43
Joined: Sun Dec 23, 2018 10:35 pm
Model of CNC Machine: X-Carve 750

45 Degree slice.

Post by W2csa »

Hi all,
I am trying to make a 8 x 10" award plaque with a .75" Ogee edge and a 4", 45 Degree cut/slice half way along the bottom edge to attach an engraved plate.
I hope this makes sense. I have a 90 Degree Vbit that is 1/2" diameter. The material is .757" thick. I would like the cut to cover the total thickness of the material.
I've tried a Vcarve tool path but that went to the whole inside. Any help would be appreciated.
Thanks
Attachments
Vectric.crv
(30 KiB) Downloaded 58 times

W2csa
Posts: 43
Joined: Sun Dec 23, 2018 10:35 pm
Model of CNC Machine: X-Carve 750

Re: 45 Degree slice.

Post by W2csa »

OK... I think I'm getting closer.
I think I need to interupt the Ogee tool path for the spot of the 45 degree slice, then make a box .757 x 4" and add a 90 Degree tool path to the box ??

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: 45 Degree slice.

Post by FixitMike »

The simple way is to make a box that is .757x2=1.514" high by 4+2x.757=5.144" wide and place it half on the edge of the material, then VCarve the box with a 90 degree bit. Half of the cuts will be in air, but it will get the job done.
plate slice.JPG
You will have to work with the ogee path until the preview shows you what you want. I got good results with a .5"ogee, but a .75" ogee cuts into the mounting surface.

Another way is to use the moulding toolpath with a ballnose bit. See Help--Help Contents for quick instructions.
Last edited by FixitMike on Wed Mar 13, 2019 9:09 pm, edited 2 times in total.
Good judgement comes from experience.
Experience comes from bad judgement.

W2csa
Posts: 43
Joined: Sun Dec 23, 2018 10:35 pm
Model of CNC Machine: X-Carve 750

Re: 45 Degree slice.

Post by W2csa »

Got it, thanks!

W2csa
Posts: 43
Joined: Sun Dec 23, 2018 10:35 pm
Model of CNC Machine: X-Carve 750

Re: 45 Degree slice.

Post by W2csa »

New question...
How can I eliminate the "V"'s on the ends so that they are straight?
Thanks

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: 45 Degree slice.

Post by FixitMike »

If you use the moulding toolpath with a ballnose bit, it will eliminate the end slopes, You will have to extend the cut beyond the edge of the material to get a flat cut. In order to do this, you will have to lie about the material thickness because the moulding toolpath won't let you cut below the bottom of the material. e.g. Set the material to 1" thick.
The plate surface will be flat except for the bit radius on the ends. You can make this smaller with a smaller radius bit, but the cutting will take longer.
Shown with 1/2" Ogee and 1" material.
Shown with 1/2" Ogee and 1" material.
Good judgement comes from experience.
Experience comes from bad judgement.

W2csa
Posts: 43
Joined: Sun Dec 23, 2018 10:35 pm
Model of CNC Machine: X-Carve 750

Re: 45 Degree slice.

Post by W2csa »

Thanks so much Mike, that's it!

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: 45 Degree slice.

Post by FixitMike »

And another option. You can use the fluting toolpath with parallel lines. Use 65 parallel lines .0625 apart with a .25 plunge cutting end mill. The lines need to be moved down an amount equal to the radius of the bit to account for the fact that the fluting toolpath specifies where the center of the bit travels.
Attachments
plate slice fluting.JPG
Good judgement comes from experience.
Experience comes from bad judgement.

W2csa
Posts: 43
Joined: Sun Dec 23, 2018 10:35 pm
Model of CNC Machine: X-Carve 750

Re: 45 Degree slice.

Post by W2csa »

Thanks mike I’ll give both a try in the morning.

Post Reply