Router Forums banner
1 - 10 of 10 Posts

·
Registered
Joined
·
1,244 Posts
Discussion Starter · #1 · (Edited)
I've been a bit obsessed lately to reduce the time a repeating project of mine takes to cut using my Probotix Meteor CNC. Thought I'd share a few of the strategies I'm exploring, with the hope that I might read a few others from the brilliant members here.
First of all this project is parts cut from a 30" x 20" sheet of 18mm Baltic Birch plywood. It includes through mortise pockets, holes for bolt shafts and countersinks for the flat head bolts to be used, pockets for cross dowels and slots for the bolts that will intersect them, and profile cuts for 6 parts that fill most of the sheet.
Strategies:
1. Use only one bit to cut the entire project. Changing and Z-zeroing bits and loading a new toolpath take time and are an opportunity for mistakes to be made (like forgetting the new file).
2. Reduce the mess made (less cleanup time) by using a 3/16" end mill rather than a 1/4" end mill.
3. Reduce the # of passes used where possible. While the default pass depth is normally 1/2 the bit diameter, I find I can set a 3/16" bit to 1/8" passes as the cross section through the wood is still 25% less to remove than for a 1/4" bit at that same depth. Then If the software wants to use 6 passes I reset it to do the toolpath in 5.
4. Tabs slow down a cut when the bit slows to hop over them. I'll use as few tabs as possible to keep the part in place during a job. Usually 3 but sometimes just two on any part perimeter. Then I'll set the tab thickness to 1/5 or less the board thickness so the toolpath only hops over tabs on the last pass.
5. Cut countersinks with the end mill. I found I can use a rotary array of short vectors and the fluting toolpath to make a decent countersink for the bolt holes. No bit change required here.
6. Reduce clearance (Z1) and plunge (Z2) and Z gap above material to .1" or less. My Z travel/plunge speed is the slowest setting for every bit I have. Reducing the time the bit rises up between passes or new vectors makes a huge reduction in total cut time.
7. Set a Home/Start position in the middle of all the cuts rather than leave it at the corner I've zeroed X and Y at.
8. Reduce as much as possible the distance the bit moves between new cuts. Merging the bolt hole pockets with the fluting chamfer cuts means the bit only travels to each bolt spot once. Strategic use of vector selection order for sequential cuts can greatly improve on the software's (Aspire) default logic for reducing overall travel time.

The first time I cut this job the CNC was busy for 27 minutes. I now have that time down to 12 minutes, and with no bit changes or post processing to be done to the parts off the CNC. Less mess to clean up before I can load another board, meaning I can usually have two done in the time it originally took me to cut one.

So what strategies have you used to reduce a project's cut time?

4D
 

·
Administrator
David - Machinist in wood
Joined
·
4,196 Posts
So what strategies have you used to reduce a project's cut time?
I switched from rectangular tabs to triangular tabs for one way to keep the tabs but not slow the machine. I think Aspire and Carveco call these 3D tabs but in Fusion 360 they're just called rectangular and triangular.

Switching to a compression bit to cut all the way through 12mm BB in one pass made a huge difference, too. When I began cutting Longworth chucks it took about 18 minutes to cut one 16" disc using a 1/4" downcut spiral at 0.125" depth of cut and 125 ipm (several passes to cut through the 12mm BB). Now I cut both discs in about 8 minutes.

Additionally, I make a rough cut in conventional leaving about 0.007" on the side walls and then follow up with a climb cut to remove not only the last 0.007" but also the tabs from the roughing cut pass. The cut is so light that it's easy to cut this leaving a very smooth finish and that has saved about 10 minutes of cleaning up all the tabs on the discs. My XY zero is always in the center on these and most other things I cut, fwiw.
 

·
Registered
Joined
·
265 Posts
like David, i also use 3d tabs .1" thick, and leave a .010" offset in climb cut. followed by a conventional clean up pass down to a .1" depth. so this leaves the tabs and a .1" step, and the cnc only has to go over the tabs once. then, while the cnc is cutting out the next parts, i take it over to the router table with a flush trim "down cut" bit and follow it around all the cuts, to remove the step and the tab remnants.

i cut the tabs off with a dremel with a small saw blade on it to prevent tearout when separating the part from the rest of the sheet.

my quest is typically for cut quality (in hardwoods), not speed. so this is all i can offer to you. but, wow, it looks like you are getting it dialed in!!!
 

·
Registered
Joined
·
1,244 Posts
Discussion Starter · #4 ·
This project is all being cut in BB plywood, or occasionally some American made birch veneer core plywood. When I'm cutting hardwood parts for my students my goal is for the best edge finish and 3D finish surface. Time is not so important for those one-off jobs.
4D
 

·
Registered
Joined
·
265 Posts
I might add to my post.

anything you can do to minimize sanding, clean-up, repairs - will play a large role in decreasing your time/piece as well. so as you approach mach speed, make sure you don't begin to suffer on quality (which I think you mentioned that its "done" as it comes off the cnc).
 

·
Registered
Joined
·
1,244 Posts
Discussion Starter · #6 ·
I have a student this semester that wanted to veneer her BB plywood parts for a quick assemble desk design. I convinced her it would be easier to veneer the plywood before we used the CNC to cut the complex shapes. Again the fine details meant using a 3/16" bit, and I set up all the through cuts to start with a downcut bit then finish with an upcut bit. We've got a couple compression bits but they are larger in diameter. No tabs were used except on the smaller parts. This was using a Multicam CNC with vacuum bed and ATC. Her parts lifted out clean and turned out great. She'll likely run a small chamfer on the crisp (sharp) edges. I could have done the chamfer on the CNC, but only on one side.

In contrast we are now on our second CNC operator, and both tend to choose speed of cut over quality of finish on the parts produced for students. Most students aren't aware the better results are possible so don't complain. I've already recut project parts for 2 students on my smaller Probotix CNCs to get a smoother finish on beveled edges and better fit on joinery details.

4D
 

·
Registered
Joined
·
1,589 Posts
I am working with a local makerspace giving CNC classes. Because we charge CNC use by the minute, it is important to give the students strategies for reducing job time. I don't think there is anything new in what we are telling them.
  • Get Feeds and Speed right
  • Minimize bit changes
  • Minimize passes
  • Reduce Z retracts
  • For V Carving go only as deep as you need
  • For general carving, hog out with big(ger) endmills, where possible.
  • Don't use bit map traced vectors if possible (LOTS of short segments)

On the last one, we push them to manually trace the image to get clean vectors. If they have to use tracing, clean up the vectors. I have seen job length cut to 1/3 with some simple clean up.

We also have them spend time looking at their toolpaths to better understand the way the CAM they are using works.
 

·
Registered
Joined
·
1,244 Posts
Discussion Starter · #8 ·
I wish we could charge our students for CNC time. Then again If I'm making the toolpaths for my students I'll favor the quality of the finished parts over the speed of the cut. That doesn't mean my toolpaths will take necessary more time, but as I know from experience there are smart strategies learned from experience that students just can't know starting out. The former shop director that is now teaching classes has added a project that is about making a chair prototype all on the CNC. As he used to oversee all the CNC jobs for the big CNC in the college fab lab he believes every student should know how to make their own toolpath files. He defends the chair project as a lesson on the value of prototypes, but then the students never follow through with a refined design based on what they learned from their CNC cut chair. Some of the CNC cut plywood chairs are reasonable, although no student admits to wishing they had a CNC cut plywood chair. Many end up abandoned and eventually thrown out. A simpler small table project could accomplish the same "make your own toolpaths" lesson and be followed up with a nice hardwood version of the table based on improvements/learned from the CNC cut plywood version.
4D
 

·
Registered
Joined
·
91 Posts
I've been a bit obsessed lately to reduce the time a repeating project of mine takes to cut using my Probotix Meteor CNC. Thought I'd share a few of the strategies I'm exploring, with the hope that I might read a few others from the brilliant members here.
First of all this project is parts cut from a 30" x 20" sheet of 18mm Baltic Birch plywood. It includes through mortise pockets, holes for bolt shafts and countersinks for the flat head bolts to be used, pockets for cross dowels and slots for the bolts that will intersect them, and profile cuts for 6 parts that fill most of the sheet.
Strategies:
1. Use only one bit to cut the entire project. Changing and Z-zeroing bits and loading a new toolpath take time and are an opportunity for mistakes to be made (like forgetting the new file).
2. Reduce the mess made (less cleanup time) by using a 3/16" end mill rather than a 1/4" end mill.
3. Reduce the # of passes used where possible. While the default pass depth is normally 1/2 the bit diameter, I find I can set a 3/16" bit to 1/8" passes as the cross section through the wood is still 25% less to remove than for a 1/4" bit at that same depth. Then If the software wants to use 6 passes I reset it to do the toolpath in 5.
4. Tabs slow down a cut when the bit slows to hop over them. I'll use a few tabs as possible to keep the part in place during a job. Usually 3 but sometimes just two on any part perimeter. Then I'll set the tab thickness to 1/5 or less the board thickness so the toolpath only hops over tabs on the last pass.
5. Cut countersinks with the end mill. I found I can use a rotary array of short vectors and the fluting toolpath to make make a decent countersink for the bolt holes. No bit change required here.
6. Reduce clearance (Z1) and plunge (Z2) and Z gap above material to .1" or less. My Z travel/plunge speed is the slowest setting for every bit I have. Reducing the time the bit rises up between passes or new vectors makes a huge reduction in total cut time.
7. Set a Home/Start position in the middle of all the cuts rather than leave it at the corner I've zeroed X and Y at.
8. Reduce as much as possible the distance the bit moves between new cuts. Merging the bolt hole pockets with the fluting chamfer cuts means the bit only travels to each bolt spot once. Strategic use of vector selection order for sequential cuts can greatly improve on the software's (Aspire) default logic for reducing overall travel time.

The first time I cut this job the CNC was busy for 27 minutes. I now have that time down to 12 minutes, and with no bit changes or post processing to be done to the parts off the CNC. Less mess to clean up before I can load another board, meaning I can usually have two done in the time it originally took me to cut one.

So what strategies have you used to reduce a project's cut time?

4D
I would say you pretty well nailed it. Once I get a repeatable project made I like to go in and tweak the settings to see if I can reduce that CNC time as well as increase quality. I found as you have after doing this I can often cut the time down by cutting multiples of the project at one time often by half by combining like toolpaths and taking a bit deeper pass often taking what software thinks would be best (vetric) and reducing those number of passes. A v60 bit takes the edges off and with a lite sanding it's ready to finish. As you know each project is specific and what were cutting can make all the difference in success or a tweak.
 

·
Registered
Joined
·
1,244 Posts
Discussion Starter · #10 ·
Another time reduction I'm contemplating, which may yield more parts per sheet of plywood, is to not use the CNC for all the straight sides of the parts. Every part is essentially a narrow rectangle. There are mortises and bolt holes cut in the center, and the short ends both have a unique profile shape. I can use my table saw to rip the plywood into part-width strips. Cut them to rough length with my radial arm saw using a stop block to make sure they are all the same length.

Then at the CNC I'd set up 3-sided traps for the parts to be clamped into. Make clamping a one-step action with a lever clamp. Run toolpaths to cut the exposed end, and whatever is within the half closest to that exposed end. Next to this part trap would be a second one, in which the parts would go head first. CNC then cuts all the details on the bottom end of the parts.

No CNC time is spent cutting the long sides of the parts. Some time is added to load and clamp successive parts.
As these parts are BB plywood, and it seems pretty good at dulling the bits I use, I'll have to consider how many parts I can cut before I need to change to a new bit. Not using the bit to cut the long sides should let it cut MORE end details before getting too dull.

4D
 
1 - 10 of 10 Posts
Top