New user and Moulding Toolpath

This forum is for general discussion about Aspire
Post Reply
mszalay
Posts: 8
Joined: Thu Jun 24, 2021 12:48 pm
Model of CNC Machine: Biesse Rover K FT

New user and Moulding Toolpath

Post by mszalay »

Hello,

I've just purchased Aspire and my first task is to make a crown moulding. I have found the Moulding Toolpath function and can take my section of the profile and create my moulding toolpath from it.

My question is:

What is the best way to use multiple tools to cut this profile? I am using a flat end mill to hog out the majority and then using a smaller ball nose to do the final pass. Since this profile has multiple sections which are at 45 degrees, I would really like to use the 45 degree bit in combination with the ball nose. It would be a better finish and save a lot of machining time as well.

Any suggestions?

Thanks

Mike

User avatar
ohiolyons
Vectric Wizard
Posts: 1702
Joined: Wed May 27, 2009 7:16 pm
Model of CNC Machine: Laguna IQ
Location: Kettering, Ohio

Re: New user and Moulding Toolpath

Post by ohiolyons »

Don't use the molding toolpath that much but I don't think you can do what you want to do with the moulding toolpath.

Moulding toolpaths are typically faster than Roughing and finish, but the moulding toolpath won't let you pick and choose areas like you want. The moulding toolpath is applied across the entire model.

The Roughing and Finishing toolpath would allow you to select areas by vectors to use you ball nose and then use a VCarve toolpath in the 90 degree areas.

I could be wrong, I hardly ever use that toolpath. It is my understanding it can be faster and sometimes smoother than Roughing and Finishing toolpaths for certain profiles.
John Lyons
CNC in Kettering, Ohio

mszalay
Posts: 8
Joined: Thu Jun 24, 2021 12:48 pm
Model of CNC Machine: Biesse Rover K FT

Re: New user and Moulding Toolpath

Post by mszalay »

John

Thanks for the reply. I will have to start looking into the program more. I just chose the moulding profile because it was very easy to take my cross section of the crown and generate the toolpath along a line.

Mike

User avatar
dealguy11
Vectric Wizard
Posts: 2464
Joined: Tue Sep 22, 2009 9:52 pm
Model of CNC Machine: Anderson Selexx 510
Location: Henryville, PA

Re: New user and Moulding Toolpath

Post by dealguy11 »

If it's crown molding, it would need to be a really big 45 degree bit to cut away the waste!

Unfortunately, the moulding toolpath doesn't use 45 degree bits for roughing. If you use an end mill for roughing, it will cut down in layers based on the depth of cut for the bit. A large end mill will speed this up, but leave more to be cut away by the carving bit.

If you want to use a 45 degree bit, you would need to set up a separate profile toolpath.

EDIT - re-reading your post, I realized you're saying the actual profile has 45-degree sections. In that case, I'd probably set up a moulding toolpath using the entire profile and run the roughing pass only. Then create one or more 45 degree profile passes at the appropriate depths. Finally, create one or more moulding toolpaths for the remainder of the profile (without roughing, since it's already done), and run those. You will need to set up the appropriate gap above the toolpath for each section. Takes a little longer to set up, but less time to run.
Steve Godding
Not all who wander (or wonder) are lost

mszalay
Posts: 8
Joined: Thu Jun 24, 2021 12:48 pm
Model of CNC Machine: Biesse Rover K FT

Re: New user and Moulding Toolpath

Post by mszalay »

I think I understand what you are saying. I created the profile as a complete closed object. In this case I would only select parts of the profile I want and choose a bit to run that portion. Then create another moulding profile based on the other portions. This sounds plausible and I'll look into it.

Thanks
Mike

User avatar
dealguy11
Vectric Wizard
Posts: 2464
Joined: Tue Sep 22, 2009 9:52 pm
Model of CNC Machine: Anderson Selexx 510
Location: Henryville, PA

Re: New user and Moulding Toolpath

Post by dealguy11 »

The profile for a moulding toolpath must be an open vector, not a closed object. That may not be what you meant, but in the Vectric software a closed vector is one where the beginning and end are connected. Sorry to be pedantic, but just want to make sure. The rail may be a closed vector, but not the profile.
Steve Godding
Not all who wander (or wonder) are lost

mszalay
Posts: 8
Joined: Thu Jun 24, 2021 12:48 pm
Model of CNC Machine: Biesse Rover K FT

Re: New user and Moulding Toolpath

Post by mszalay »

Steve,

No worries I appreciate the details. In this case, perhaps I was lucky, the closed vector worked fine. The moulding toolpath seemed to ignore anything that would be under cut. This was just in a simple straight line rail, perhaps in a more complicated rail shape I may run into problems. I will certainly keep this in mind, If I had not have imported this shape from my other software I would not have drawn the complete closed shape.

Thanks again for the help.

Mike

4DThinker
Vectric Wizard
Posts: 1701
Joined: Sun Sep 23, 2012 12:14 pm
Model of CNC Machine: CNC Shark Pro, Probotix Meteor 25" x 50"

Re: New user and Moulding Toolpath

Post by 4DThinker »

You can break up the moulding profile into sections, then use the V Bit with the profile toolpath to cut the 45 degree section. When I've got a moulding toolpath that has sharp corners I generally leave those to an endmill or v-bit with a profile toolpath and let a ball nose bit do all the curvy sections with the moulding toolpath.
4D

User avatar
adze_cnc
Vectric Wizard
Posts: 4325
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: New user and Moulding Toolpath

Post by adze_cnc »

mszalay wrote:
Mon Jun 28, 2021 3:35 pm
What is the best way to use multiple tools to cut this profile?
Were you going to attach an image of “that” profile?

mszalay
Posts: 8
Joined: Thu Jun 24, 2021 12:48 pm
Model of CNC Machine: Biesse Rover K FT

Re: New user and Moulding Toolpath

Post by mszalay »

I can. I have a better understanding now. Here is the first moulding I made. Pretty standard crown but I needed in Rift Oak and asap and 12 ft long. It took 1.5hrs to cut, so next time I'm trying to find ways to improve on the speed. The quality was surprisingly really good for just a 1/4" ball nose bit and flat endmill. I was impressed with the flat 45 degree sections but next time using a 45 bit will be better.
Screenshot 2021-06-29 114510.png

User avatar
adze_cnc
Vectric Wizard
Posts: 4325
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: New user and Moulding Toolpath

Post by adze_cnc »

mszalay wrote:
Tue Jun 29, 2021 4:50 pm
but next time using a 45 bit will be better.
Here's where your image clarified something I was unsure of.

V-bits (those that in theory come to a mathematical point with no flat) are set up in Vectric programs (and usually quoted by manufacturers) using the total included angle. So, 90 degrees in the case of a bit whose one side is 45 degrees from the vertical.

But, engraving bits (angled bits that do have a flat even if it is only 0.001 inches) are specified using the side angle only. So, a 45 degree engraving bit is one that would be entered as a 90 degree v-bit if it had no flat.

Because of this when I saw 45-bit I was expecting something with a 22.5 deg side angle. Something you might use if you were cutting slats for an octagon.

What's the height (or width) of the moulding? I thought this might be a nice practice piece for disassembling a profile into multiple mixed toolpaths (moulding and profile).

mszalay
Posts: 8
Joined: Thu Jun 24, 2021 12:48 pm
Model of CNC Machine: Biesse Rover K FT

Re: New user and Moulding Toolpath

Post by mszalay »

I will have to watch my terminology and thanks for the explanation.

I would love to see how someone with Aspire experience handle this. My cad/cam software is a lot different and can not do half what Aspire can. (At least not with out spending crazy amounts of money on modules, hence why I have purchased Aspire).

This crown is 4.25” wide, 3/4” thick. It has a spring angle of 45 degrees.

Thanks

Mike

User avatar
adze_cnc
Vectric Wizard
Posts: 4325
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: New user and Moulding Toolpath

Post by adze_cnc »

Test file, made with VCarve, containing 5 toolpaths:
  • 3 profile paths "on the line" using 90 deg v-bit to cut top, bottom, and middle "chamfers" (v9.519 does not have the chamfer toolpath)
  • 2 separate moulding paths to cut the 2 curved portions separated by the "chamfers"
I was going to use a 1/4" ball end cutter but I changed my mind and went with a 3/8" one as that's my go to one "in real life". With a robust ball end bit and how the curves are cut I wouldn't bother with the square end bit to rough out things.

The feed rates, spindles speeds, and rapid move rate are for my machine if I could do a 12-foot long piece.

The step over for the moulding ball end cutter is set at 0.05 inches. If this were Douglas Fir, MDF, or similar I'd accept 0.0625 inches. But for beech, normal oak, birch plywood, etc. I'd be happy with 0.05 inches.

Note the moulding profile in layer "m_profile and rail 1". The hook up is to prevent the ball end cutter from digging into the flat face of the "middle" chamfer while still allowing it to blend into the flat area on the other face.

For the chamfers on the bottom of the board I'd use a tablesaw or router table.

If you want to do them in Aspire you could make this a double-sided project. Copy the contents of layers "chamfer top" and "chamfer bottom" to the bottom side. Then create toolpaths (profile "on the line" or chamfer in version 10.x) to cut them to the proper depths.
Attachments
moulding test.crv
VCarve v9.519
(78 KiB) Downloaded 50 times

mszalay
Posts: 8
Joined: Thu Jun 24, 2021 12:48 pm
Model of CNC Machine: Biesse Rover K FT

Re: New user and Moulding Toolpath

Post by mszalay »

Thanks for this. I will look at it a little further when I get a little more time.

The under side chamfers are done on the shaper for sure. I would normally use the shaper to do this whole profile in 1-2 passes but when I only need a small piece and can't wait for the knife to be made for a random size, the CNC is a great option.

The piece I ran used a step of .025" and the result was pretty nice. I may try to step that out a little more next time. The larger ball nose might be key too. Certainly when the chamfers can be done with a 90 degree :) bit.

Mike

Post Reply