Tapered Hole
-
- Vectric Apprentice
- Posts: 53
- Joined: Fri May 01, 2009 5:05 pm
Tapered Hole
I need to cut a tapered hole for a router holder and cant seem to figure out how to do it. It will be cut into ¾ oak and the hole needs to be 2.47 inches at the top and 2.35 at the bottom. I created a model using the two rail sweep, but because the taper is so small I couldn’t get it to cut correctly. Is there a way to cut it using the pocket option?
Thanks,
Richard
Thanks,
Richard
-
- Vectric Wizard
- Posts: 4797
- Joined: Thu May 18, 2006 3:24 pm
- Model of CNC Machine: ShopBot
- Location: North Carolina
Re: Tapered Hole
Richard,
How smooth do the sides have to be?
Tim
How smooth do the sides have to be?
Tim
-
- Vectric Apprentice
- Posts: 53
- Joined: Fri May 01, 2009 5:05 pm
Re: Tapered Hole
Tim,
If the taper is close, I can probably hand sand to get it smooth.
Richard
If the taper is close, I can probably hand sand to get it smooth.
Richard
-
- Vectric Wizard
- Posts: 4797
- Joined: Thu May 18, 2006 3:24 pm
- Model of CNC Machine: ShopBot
- Location: North Carolina
Re: Tapered Hole
Richard,
Machining near vertical sides with 3D toolpaths are a challenge.
My thoughts when I read this was to create a series of 2D toolpaths which would leave a ridged surface, which is why I asked the question.
Take a look at this and see if it interests you. It takes longer to set up than cut, but even the setup time isn't bad. For speed I created toolpaths 0.125" apart in Z, you could easily make these closer together which would improve the surface.
I started with an exact size vector representing the side view of you hole. Then drew a horizontal line and used to array copy tool to create an array of horizontal lines. Then used the trim tool to trim each line to the tapered side. These lines represent the diameter for a 2D Profile-Inside toolpath as well as the Cut Depth.
The center was first 'hogged' out with a pocket toolpath. Then individual Profile-Inside toolpaths created for each step. Once setup, assuming you used the same bit, all the toolpaths could be saved as one to cut on your machine. The total time estimate for my CNC was less than 1 minute.
If you need or want more detail, let me know.
Tim
Machining near vertical sides with 3D toolpaths are a challenge.
My thoughts when I read this was to create a series of 2D toolpaths which would leave a ridged surface, which is why I asked the question.
Take a look at this and see if it interests you. It takes longer to set up than cut, but even the setup time isn't bad. For speed I created toolpaths 0.125" apart in Z, you could easily make these closer together which would improve the surface.
I started with an exact size vector representing the side view of you hole. Then drew a horizontal line and used to array copy tool to create an array of horizontal lines. Then used the trim tool to trim each line to the tapered side. These lines represent the diameter for a 2D Profile-Inside toolpath as well as the Cut Depth.
The center was first 'hogged' out with a pocket toolpath. Then individual Profile-Inside toolpaths created for each step. Once setup, assuming you used the same bit, all the toolpaths could be saved as one to cut on your machine. The total time estimate for my CNC was less than 1 minute.
If you need or want more detail, let me know.
Tim
- Attachments
-
- Tapered hole with 2D toolpaths.crv
- (191.5 KiB) Downloaded 262 times
- mezalick
- Vectric Wizard
- Posts: 2970
- Joined: Mon Nov 03, 2008 9:07 am
- Model of CNC Machine: Camaster Cobra
- Location: Philadelphia, PA USA
- Contact:
Re: Tapered Hole
I came up with 4.5 degrees on each side.
Maybe you can use a tappered bit to solve this problem.
Michael
Maybe you can use a tappered bit to solve this problem.
Michael
Michael Mezalick
https://www.youtube.com/user/mezalick
mm@mezalick.com
https://www.youtube.com/user/mezalick
mm@mezalick.com
-
- Vectric Craftsman
- Posts: 277
- Joined: Sat Mar 29, 2008 8:00 pm
- Location: Millington, MI
- Contact:
Re: Tapered Hole
Michael,
I used the Create Shape from Vector.
Stock= .750" thick 5"x5"
Hole dia= . 2.47" larger dia.
See attached screen shots, I set it at 86.5 deg = 7 deg included. You will want to set the angle at 85.5 deg to equal 4.5 deg taper per side.
I then used a hole profile toolpath, leave some stock for finish sanding.
the smaller depth per the better finish you will get,
Hope this works for you, it did when I needed approx the same profile.
Buck
I used the Create Shape from Vector.
Stock= .750" thick 5"x5"
Hole dia= . 2.47" larger dia.
See attached screen shots, I set it at 86.5 deg = 7 deg included. You will want to set the angle at 85.5 deg to equal 4.5 deg taper per side.
I then used a hole profile toolpath, leave some stock for finish sanding.
the smaller depth per the better finish you will get,
Hope this works for you, it did when I needed approx the same profile.
Buck
-
- Vectric Apprentice
- Posts: 53
- Joined: Fri May 01, 2009 5:05 pm
Re: Tapered Hole
Tim,
Had to let it sink in, but I understand what you are doing. If I make .0625 passes and use a 1/8 tapered bit, like Michael suggested, it should leave the sides fairly smooth.
Thanks to everyone for you input.
Richard
Had to let it sink in, but I understand what you are doing. If I make .0625 passes and use a 1/8 tapered bit, like Michael suggested, it should leave the sides fairly smooth.
Thanks to everyone for you input.
Richard
- sawmiller
- Vectric Wizard
- Posts: 531
- Joined: Sat May 03, 2008 8:34 pm
- Model of CNC Machine: joe's rack and pinion hybrid
- Location: camden,tn
Re: Tapered Hole
tim, couldnt you create a tool with the required taper on the sides, do a pocket, then create componet from preview ?
might try this when i'm not on my way to work
might try this when i'm not on my way to work
woodmizer sawmill and joe's hybrid cnc, a good combination
In the heart of Tn
In the heart of Tn
-
- Vectric Wizard
- Posts: 4797
- Joined: Thu May 18, 2006 3:24 pm
- Model of CNC Machine: ShopBot
- Location: North Carolina
Re: Tapered Hole
Hi Dan,
Yes, that method would work great but you would still end up with a 3D component needing to be cut with 3D toolpaths. The issue here, as I understood it, was not how to model it but cut it using 2D toolpaths. Ideal way would be a custom made bit with the correct side angle but cost would be significant.
Tim
Yes, that method would work great but you would still end up with a 3D component needing to be cut with 3D toolpaths. The issue here, as I understood it, was not how to model it but cut it using 2D toolpaths. Ideal way would be a custom made bit with the correct side angle but cost would be significant.
Tim
Re: Tapered Hole
I didn't want to over exert my brain,( I have to conserve has much I got left), so I used another cad software, in my case I used Rhino, drew the profile then imported into Aspire as a 3ds file. The whole process took less than a minute. On the preview, I used a ball-nose mill and it seemed to work fine.
-
- Vectric Wizard
- Posts: 4797
- Joined: Thu May 18, 2006 3:24 pm
- Model of CNC Machine: ShopBot
- Location: North Carolina
Re: Tapered Hole
The issue is not modeling it. Aspire will do that perfectly and no other software is required.
The issue is the real world challenge of the actual machining of vertical or near vertical surfaces with a 3D finish pass and ending up with an acceptable surface cut quality.
Tim
The issue is the real world challenge of the actual machining of vertical or near vertical surfaces with a 3D finish pass and ending up with an acceptable surface cut quality.
Tim
Re: Tapered Hole
You got me curious, so I tried my design using a 6mm ball mill for the finish toolpath. Not only was the taper very actuate, the finish was okay, but would of been better if I used a smaller stepover. That showed me I don't need a special tool for a taper and using another cad software with Aspire sped things up so I could get into production alot faster.
-
- Vectric Wizard
- Posts: 4797
- Joined: Thu May 18, 2006 3:24 pm
- Model of CNC Machine: ShopBot
- Location: North Carolina
Re: Tapered Hole
It is always best when you can take it to the machine.
Good job!
Good job!
-
- Vectric Apprentice
- Posts: 53
- Joined: Fri May 01, 2009 5:05 pm
Re: Tapered Hole
Tim,
I should have posted a follow up earlier, but I cut the taper using your approach and it worked fine. I created 12 2D tool paths and set each to cut .0625 using a 1/8 tapered ball nose. I saved all the tool paths together as one file. The only thing I didn't understand was that after each tool path would finish, it would start back at the top and retrace each previously cut path until it reached the next path that was due to be cut. I would have thought that since they were individual tool paths that it would have cut from top to bottom without retracing the previously cut paths. ??
At any rate, the taper was correct and it left a nice finish.
Thanks for the help.
I should have posted a follow up earlier, but I cut the taper using your approach and it worked fine. I created 12 2D tool paths and set each to cut .0625 using a 1/8 tapered ball nose. I saved all the tool paths together as one file. The only thing I didn't understand was that after each tool path would finish, it would start back at the top and retrace each previously cut path until it reached the next path that was due to be cut. I would have thought that since they were individual tool paths that it would have cut from top to bottom without retracing the previously cut paths. ??
At any rate, the taper was correct and it left a nice finish.
Thanks for the help.
-
- Vectric Wizard
- Posts: 4797
- Joined: Thu May 18, 2006 3:24 pm
- Model of CNC Machine: ShopBot
- Location: North Carolina
Re: Tapered Hole
Hi Richard,
Thanks for the update and happy it worked for you.
I'm thinking what you saw for the toolpaths was the Pass Depth being set less than the Cut Depth. If you set the Pass Depth to 0.75" for all the toolpaths, then you should see a single pass to each Cut Depth.
Tim
Thanks for the update and happy it worked for you.
I'm thinking what you saw for the toolpaths was the Pass Depth being set less than the Cut Depth. If you set the Pass Depth to 0.75" for all the toolpaths, then you should see a single pass to each Cut Depth.
Tim