45 Degree slice.

This forum is for general discussion regarding VCarve Pro

45 Degree slice.

Postby W2csa » Wed Mar 13, 2019 7:15 pm

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 21 times
W2csa
 
Posts: 28
Joined: Sun Dec 23, 2018 10:35 pm
Model of CNC Machine: X-Carve 750

Re: 45 Degree slice.

Postby W2csa » Wed Mar 13, 2019 7:28 pm

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 ??
W2csa
 
Posts: 28
Joined: Sun Dec 23, 2018 10:35 pm
Model of CNC Machine: X-Carve 750

Re: 45 Degree slice.

Postby FixitMike » Wed Mar 13, 2019 9:03 pm

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.
User avatar
FixitMike
Vectric Wizard
 
Posts: 1500
Joined: Sun Apr 17, 2011 5:21 am
Location: Renton, WA USA
Model of CNC Machine: Shark Pro Plus (modified)

Re: 45 Degree slice.

Postby W2csa » Wed Mar 13, 2019 9:06 pm

Got it, thanks!
W2csa
 
Posts: 28
Joined: Sun Dec 23, 2018 10:35 pm
Model of CNC Machine: X-Carve 750

Re: 45 Degree slice.

Postby W2csa » Wed Mar 13, 2019 9:36 pm

New question...
How can I eliminate the "V"'s on the ends so that they are straight?
Thanks
W2csa
 
Posts: 28
Joined: Sun Dec 23, 2018 10:35 pm
Model of CNC Machine: X-Carve 750

Re: 45 Degree slice.

Postby FixitMike » Wed Mar 13, 2019 9:42 pm

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.
plate slice moulding.JPG
Shown with 1/2" Ogee and 1" material.
Good judgement comes from experience.
Experience comes from bad judgement.
User avatar
FixitMike
Vectric Wizard
 
Posts: 1500
Joined: Sun Apr 17, 2011 5:21 am
Location: Renton, WA USA
Model of CNC Machine: Shark Pro Plus (modified)

Re: 45 Degree slice.

Postby W2csa » Wed Mar 13, 2019 9:50 pm

Thanks so much Mike, that's it!
W2csa
 
Posts: 28
Joined: Sun Dec 23, 2018 10:35 pm
Model of CNC Machine: X-Carve 750

Re: 45 Degree slice.

Postby FixitMike » Wed Mar 13, 2019 10:13 pm

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.
User avatar
FixitMike
Vectric Wizard
 
Posts: 1500
Joined: Sun Apr 17, 2011 5:21 am
Location: Renton, WA USA
Model of CNC Machine: Shark Pro Plus (modified)

Re: 45 Degree slice.

Postby W2csa » Wed Mar 13, 2019 10:40 pm

Thanks mike I’ll give both a try in the morning.
W2csa
 
Posts: 28
Joined: Sun Dec 23, 2018 10:35 pm
Model of CNC Machine: X-Carve 750


Return to VCarve - General

Who is online

Users browsing this forum: WNC_Ed and 10 guests