Upcut-/Downcut- or Compression-Bit for Clean Cutting Edges?

Post Reply
halodri
Vectric Apprentice
Posts: 55
Joined: Tue Jul 26, 2022 11:42 am
Model of CNC Machine: BZT PFK 1607 PX

Upcut-/Downcut- or Compression-Bit for Clean Cutting Edges?

Post by halodri »

I'm a member of a "makerspace" in Vienna/Austria with two CNC machines and I'm fairly new to CNC machining.

I want to cut and machine ( 27mm glued laminate timber)several pieces for furniture and I'm concerned with getting nice clean edges on the top and bottom.

I've read and also my experience so far is that upcut bits tend to rip out wood on the top surface (particularly plywood) but not on the bottom and with downcut bits it's the other way around.

I know there is a combination of up and down cut bits called the compression bit.
Now I'm wondering, what's the best method/practice to achieve clean cutting edges on top and bottom. Is it better/safer to use a downcut bit for the top surface first and switch "in the middle" to an upcut bit, or does a compression bit achieve equally good results?
Capture.JPG
Hello,

User avatar
Adrian
Vectric Archimage
Posts: 14544
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: Upcut-/Downcut- or Compression-Bit for Clean Cutting Edges?

Post by Adrian »

Compression bit would do what you want but you need to use the lead-in feature of the profile toolpath to make sure the bit is at the correct depth before doing the actual cut otherwise the upcut portion on the bottom of the bit will tear the material at the start of the cut.

Otherwise you can get excellent results using two separate bits as you suggest it just takes longer.

halodri
Vectric Apprentice
Posts: 55
Joined: Tue Jul 26, 2022 11:42 am
Model of CNC Machine: BZT PFK 1607 PX

Re: Upcut-/Downcut- or Compression-Bit for Clean Cutting Edges?

Post by halodri »

Hello Adrian,

Thanks for your answer. I've now watched a few videos on how compression bits work. My understanding is that the path depth of the first path must exceed the length of the upcut portion of the bit. otherwise only the upcut portion is acting and thus rips out material on the surface.

I ordered this compression bit from Amazon:

https://www.amazon.de/SpeTool-Upwards-M ... ompression+ bit +6mm%2Cindustrial%2C109&sr=1-1-spons&psc=1

However, I could not find any information about the length of the upcut part of the bit. It looks like it's around 6mm long. Assuming it's really 6mm long. Does that mean the first path has to be 7mm deep? I ask because 7mm seems a lot, especially in hardwood. I always use the default Vcarve cutting parameters and from what I remember the path depth is usually around 2mm in hardwood.

User avatar
Adrian
Vectric Archimage
Posts: 14544
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: Upcut-/Downcut- or Compression-Bit for Clean Cutting Edges?

Post by Adrian »

Yes, the first pass has to be lower than the upcut section, that's why you need the lead-in as well otherwise the plunge/ramp will tear the material surface.

Pass depths depend a lot on the machine. 7mm or more shouldn't be a problem for a machine meant for cutting cabinet parts (if that's what you have). I cut up to 18mm MDF, chipboard, plywood and softwoods in a single pass all the time. Hardwoods I rarely do but when I do it's a couple of passes unless it's something really dense.

The defaults in VCarve are just placeholders really. They are ultra-safe settings that shouldn't damage lightweight desktop machines. You should always adjust the settings for the machine/material/bit combination you are using for optimal results. That is the biggest learning curve of CNC in my experience. Learning what the machines are actually capable of.

halodri
Vectric Apprentice
Posts: 55
Joined: Tue Jul 26, 2022 11:42 am
Model of CNC Machine: BZT PFK 1607 PX

Re: Upcut-/Downcut- or Compression-Bit for Clean Cutting Edges?

Post by halodri »

Adrian wrote:
Sun Oct 09, 2022 9:53 am
I cut up to 18mm MDF, chipboard, plywood and softwoods in a single pass all the time.
Ok, "18mm all the time" caught my interest.So far I haven't given much thought to things like path depth since I was busy enough to get a good enough Vectric file and get the machine up and running at all.

https://wiki.happylab.at/w/CNC_Fr%C3%A4 ... Fraese.jpg
Adrian wrote:
Sun Oct 09, 2022 9:53 am
The defaults are ultra-safe settings that shouldn't damage lightweight desktop machines.
I have now done some research and the manufacturer of the machine provides a cutting data calculator and it says with a 6mm bit I can cut a slot in hardwood/plywood with a depth of 6mm and in softwood of up to 12mm. This seems close to the values you have mentioned.
Capture.PNG
Ok, now I am better informed. Thanks for taking the time to answer Andrian!

Seems lile the next thing on my list is to educate myself on a "lead-in". I have never used that befor.

User avatar
Burnside
Posts: 44
Joined: Wed Sep 07, 2022 10:39 pm
Model of CNC Machine: ShopSabre

Re: Upcut-/Downcut- or Compression-Bit for Clean Cutting Edges?

Post by Burnside »

Not sure on the OP but the compression bits I use are meant to plunge directly at the changeover depth (the point where it goes from up -> down cut). I recommend not use a lead in or you'll get a little tearout as the bit progresses to depth. As mentioned, the pass depth of the first pass must be greater than the changeover. I usually add .05 or so to be sure I'm past the chaneover depth and I setup my tool database so that the pass depth is equal to this value, so I can quickly setup the toolpath.

User avatar
Adrian
Vectric Archimage
Posts: 14544
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: Upcut-/Downcut- or Compression-Bit for Clean Cutting Edges?

Post by Adrian »

Burnside wrote:
Tue Jan 31, 2023 10:23 pm
I recommend not use a lead in or you'll get a little tearout as the bit progresses to depth.
Lead in and outs are made in the waste side so the tearout doesn't matter.

User avatar
FabLab Wageningen
Vectric Craftsman
Posts: 210
Joined: Mon May 09, 2022 8:17 pm
Model of CNC Machine: Ooznest Workbee 1500x1500
Location: Wageningen, Netherlands
Contact:

Re: Upcut-/Downcut- or Compression-Bit for Clean Cutting Edges?

Post by FabLab Wageningen »

Your reference to the bit you bought does not work, unfortunately.

But a generic rule-of-thumb is that the longer the cutting height of the compression bit is and the larger the shank diameter is, the larger the 'upcut' part will be. For a normal 6 mm diameter shank I would reckon a 6 mm 'upcut' part is likely, but when you want to cut through a whopping 27 mm sheet you need a bit with quite a long cutting height. Looking at the Amana catalog, for example, I see only one bit that has a 28 mm cutting height (48322-K) and that has a 9 mm 'upcut' part, so you need a first pass of 9,2 mm. Can your machine handle that ?

Marcel.

User avatar
Burnside
Posts: 44
Joined: Wed Sep 07, 2022 10:39 pm
Model of CNC Machine: ShopSabre

Re: Upcut-/Downcut- or Compression-Bit for Clean Cutting Edges?

Post by Burnside »

Adrian wrote:
Wed Feb 01, 2023 10:10 am
Burnside wrote:
Tue Jan 31, 2023 10:23 pm
I recommend not use a lead in or you'll get a little tearout as the bit progresses to depth.
Lead in and outs are made in the waste side so the tearout doesn't matter.
Apologies, my brain read ramp in :? You are correct. That is a good way if you have the room from clamps and enough waste material. Cheers

halodri
Vectric Apprentice
Posts: 55
Joined: Tue Jul 26, 2022 11:42 am
Model of CNC Machine: BZT PFK 1607 PX

Re: Upcut-/Downcut- or Compression-Bit for Clean Cutting Edges?

Post by halodri »

I learned a lot about compression bits and how they should be used from all the helpful comments. I've completed my project and found that I didn't need to use compression bits.

On the one hand I don't like using lead ins and outs as it wastes a bit more material. But more important, they are not suitable for "do separate last path" to create a nice edge, because a groove is created in the transition area between the up and down cut section. So, I ended up using mostly a down cut bit: drilling narrow 8mm pocket holes for dowels, cutting from the top surface all the way to the bottom and for " do separate last path".

At first, I was worried about chip clearance problems with down cut bits, especially when drilling 8mm dowel holes in 27mm boards with a 6mm bit, and also bottom tear out. But I haven't had any issues like that. There have been no burn marks or smoke at the dowel holes. Since the wooden boards are held to the waste board at the bottom, the down cut bit doesn't cause bottom tear out. Based on this, I plan to stick to using only down cut bits in the future.

This is the image gallery for my project if you are interested. (I haven't had time to organize and reduce the number of images yet, hence chaos and way too many images :lol: ):

https://photos.app.goo.gl/UokauNTRRb42GED27

Post Reply