kyokahn

DIY cheap CNC - Test cut successful!

Recommended Posts

Well I'm impressed! Can't wait to see it cutting once you get it tuned re accelerations and velocities. Great idea on the torsion boxes.

Curious what the 'popcorn' noise is in the videos.

 

  • Like 1

Share this post


Link to post
Share on other sites
4 hours ago, Mick S said:

Well I'm impressed! Can't wait to see it cutting once you get it tuned re accelerations and velocities. Great idea on the torsion boxes.

Thanks! I'll try to give it a spin this weekend.

4 hours ago, Mick S said:

Curious what the 'popcorn' noise is in the videos.

Popcorn noise is actually water falling on the garage roof, from a leaky gutter on the balcony after a storm. Most houses here have metal roofing so it's like a giant drum some times.

Share this post


Link to post
Share on other sites

Well, finally! First cuts are here. I pushed the acceleration a bit and kept the rapid speed.

  • Rapid speed 4000mm/m
  • Acceleration (grbl-no curve) 50mm/s/s
  • Feed 2500mm/m (100ipm)
  • 1/8 flat endmill - 12000 rpm - 2mm per pass - 2mm stepover
  • adaptive mode + helix entry

And a couple shots 

20180217_193621_HDR.jpg


20180217_193633_HDR.jpg

The good:

  • 2 pockets 5mm deep in around 6 minutes. Fast enough considering the type of operation.
  • No dust! Shavings is what I expected. Which translates to...
  • No overheating! Bit was cold right after it was done
  • Flat bottom = tramming is accurate! (thanks wixey angle gauge!)
  • No vibration or deflection, no steps skipped and steppers barely at room temp = nema 17s are surprisingly good enough for this
  • Difference in diameter from the f360 model to the actual pice= 0.4mm. Difference in diameter from X to Y direction = under 0.1mm
  • Spindle is crazy quiet

 

The bad:

  • when fully accelerated, it vibrates a little at the bit, meaning it's almost exceeding the chip load so...
  • the spindle's 12k rpm limit proved to be the limiting factor for the build, at least with 1/8 bits. I'll test 1/4 bits later where the limiting factor will likely be the spindle's own torque (.8 hp isn't very strong)
  • no mounting setup yet
  • ghetto cables! waiting for my cheapo drag chains
  • need dust collection!

 

The ugly:

  • bed isn't flat... though at least i know it won't bend anymore due to the construction
  • need to add a waste board with mounting options... and then flatten it. It will take a while
  • forgot to grease the rails and lead screws before running it (do-oh!)

 

So there it is! If you can think of something I can do to make the build better, or if you think the feeds/cutting strategy/tool paths have something wrong, do tell! I'm pretty lost, especially in the CAM side of things.

  • Like 2

Share this post


Link to post
Share on other sites

What software are you using? Also when hogging out material like that I would go more aggressive on the depth per pass and save about .010" as a final pass depth for cleanup.

What kind of end stops are you using for homing the 0,0 location (I would assume mechanical wire switches or hall effect sensors) and what are you using for setting the length of the bit to zero the table?

As for a spoilboard, I use LDF(i have a vacuum table) and a fly cutter to make it flat in regards to the gantry geometry.

For feeds and speeds it is a lot of trial and error, you are correct that the bit should not be scalding hot, but the fact it was cool to the touch means you can be more aggressive with your feeds and speeds. Ultimately the bit should be warm to the touch, not uncomfortably so though.

I think the biggest limiting factor you have currently is the router itself with a 12kRPM limit and the collets you have. If it is only 1/8th" I would look into getting a 1/4" collet, if it is available, as there is a wider variety of 1/4" shank tooling out there.

And for cutting strategy I've only used the helical cutting for milling metals, I would use a more basic strategy depending on which software you're using that would only move either the X or the Y one at a time. Reason being having both moving at the same time without a rock solid frame can cause some backlash and vibration due to the NEMA 17's ramping up and down the power to both X and Y at the same time.

I may have just dumped a lot of information on you and I apologize if it is a bit scattered. But feel free to ask any questions!

  • Like 1

Share this post


Link to post
Share on other sites
On ‎2‎/‎25‎/‎2018 at 10:01 AM, Catco said:

What software are you using?

F360, V-Carve, UGS

On ‎2‎/‎25‎/‎2018 at 10:01 AM, Catco said:

Also when hogging out material like that I would go more aggressive on the depth per pass and save about .010" as a final pass depth for cleanup.

The spindle is the weak point for now, since it's only 500w and 12k RPM. I do have 1/4" collets and a few bits from the router, but I wouldn't think that spindle can handle a fly cutter all that well, right? 

I can go up to 1/4" deep with the 1/8" but that risks breaking the bit so I stay at around the bit's diameter for stepdown.

On ‎2‎/‎25‎/‎2018 at 10:01 AM, Catco said:

And for cutting strategy I've only used the helical cutting for milling metals, I would use a more basic strategy depending on which software you're using that would only move either the X or the Y one at a time. Reason being having both moving at the same time without a rock solid frame can cause some backlash and vibration due to the NEMA 17's ramping up and down the power to both X and Y at the same time.

You're absolutely right! Though the machine itself is quite solid, the base it rests on wiggles when doing the helical entry. I changed to ramp or Z. Vibration hasn't been an issue, but the steppes still create some resonance. Backlash though... that remains an issue, as I can't use climb cutting unless I eliminate backlash almost entirely. I'll try some anti-backlash nuts later on, for now, I'll have to stick to conventional.

 

On ‎2‎/‎25‎/‎2018 at 10:01 AM, Catco said:

What kind of end stops are you using for homing the 0,0 location (I would assume mechanical wire switches or hall effect sensors) and what are you using for setting the length of the bit to zero the table?

Mechanical switches

On ‎2‎/‎25‎/‎2018 at 10:01 AM, Catco said:

I may have just dumped a lot of information on you and I apologize if it is a bit scattered. But feel free to ask any questions!

That's great, actually! Any other ideas on how to reduce backlash?

Share this post


Link to post
Share on other sites
1 hour ago, kyokahn said:

The spindle is the weak point for now, since it's only 500w and 12k RPM. I do have 1/4" collets and a few bits from the router, but I wouldn't think that spindle can handle a fly cutter all that well, right? 

The spindle is definitely a major weak point at the moment. I've known a lot of DIY CNC's to use a Bosch or DeWalt router as the spindle to get at least 1.5HP and a variable speed setting from them. As for the fly cutter, they do make them with a 1/4" shank, but you'd currently be very limited in how fast and deep you could go per pass. but ideally you'd only want to take off .005"-.010" to get the bed flat and co planar with the gantry.

1 hour ago, kyokahn said:

You're absolutely right! Though the machine itself is quite solid, the base it rests on wiggles when doing the helical entry. I changed to ramp or Z. Vibration hasn't been an issue, but the steppes still create some resonance. Backlash though... that remains an issue, as I can't use climb cutting unless I eliminate backlash almost entirely. I'll try some anti-backlash nuts later on, for now, I'll have to stick to conventional.

Being that you're using leadscrews, the quality of them is the primary source of the backlash. Ideally you would use ballscrews as they were developed specifically for CNC applications and they minimize backlash. But getting a good quality ACME leadscrew you can expect a backlash of say .005" to start, but as time goes on it can quickly increase to .025".

Best option is either a rolled ballscrew or a ground one. With a good quality rolled ballscrew you can expect a backlash of about .003", whereas with a poorly made one about .010". A good quality ground ballscrew you can expect to see a back lash of .001" or more often less. Below is a example of how they are graded in quality:

C0 – 3um or 0.0001″ per 300 mm / 12″
C3 – 7um or 0.00027″ per 300 mm / 12″
C5 – 14um or 0.0005″ per 300 mm / 12″

This refers to how close the position will be after the screw has turned through 12″ of motion. Note that in this small of an area, there are ACME screws available that are every bit as accurate, so the ballscrew has no special advantage here over relatively short distances. But when you start increasing the speed of traverses the backlash will translate down the length of the lead screw

But it all depends on budget, some delrin antibacklash nuts can definitely help and almost eliminate backlash, but most often if the control software you're using has the ability to slow down when entering corners, used in conjunction with anti backlash nuts, should almost eliminate any backlash. But not all control software has that capability.

Do you have endstops on both the max and min for the X,Y, and Z axis?

One issue I've run into with backlash is that the gantry is a lot of times out of square with itself and with the steppers related to the positioning of the mechanical end stops. The process I use to square it all up is as follows based on the pictures I could see of your CNC:

1: Loosen the bolts connecting the bearing cars on the X(Long) axis. Loosen them to the point the gantry can pivot ever so slightly.

2: With the NEMAs unpowered, move the Y axis to about the center point of the gantry.

3: If you're using G-Code send it a G28 X ; command to home the X-axis. Or use your machine control software to find the absolute home reference point.

4: Tighten one screw on a bearing car, tightening the same screw on the opposite side pf the gantry.

5: Jog the gantry to the far end of the X axis.

6: Repeat step 3.

7: Repeat step 4.

8: Repeat step 5, and continue to do this until all the bearing car bolts are tight, but not overly so.

 

Also I would recommend single or double spiral upcut bits, they allow you to cut faster as they pull the material that is being cut up and away from the part and clear the cutting path. The only time I use 0 flute or straight bits is when I am cutting acrylic and need a mostly polished edge. But most often I use the 150W laser.

And once again I dropped a lot of information... Sorry.

  • Like 1

Share this post


Link to post
Share on other sites

Interesting on the upcut bits; I use a 1/4" spiral downcut bit 90% of the time for pockets, cutting outer profiles, etc. and I don't have an issue with chips being in the way.  But I also have a clean top edge with no fuzz or splinters.

And I guess I'm a bit conservative in DOC.  I rarely take more than 3/32" depth with a 1/8" bit and feed is usually around 75 ipm.  I cut with the 1/4" bit at 125 ipm, sometimes higher and sometimes lower.

Your machine is looking very good, btw!  I like it.

David

  • Like 1

Share this post


Link to post
Share on other sites
1 hour ago, difalkner said:

Interesting on the upcut bits; I use a 1/4" spiral downcut bit 90% of the time for pockets, cutting outer profiles, etc. and I don't have an issue with chips being in the way.  But I also have a clean top edge with no fuzz or splinters.

And I guess I'm a bit conservative in DOC.  I rarely take more than 3/32" depth with a 1/8" bit and feed is usually around 75 ipm.  I cut with the 1/4" bit at 125 ipm, sometimes higher and sometimes lower.

The machine I run at work, the slowest I go is 175ipm, most often I am cutting materials that at minimum 3-4" thick so I use the upcut bits when I need only one good face and need to clear the chips from the cut path, and I use spiral compression bits when I need both faces finished and tearout free. The smallest bit I use during normal operation is 1/2", 2" CEL.

 

Edit: When I do cut with the 1/8th bit I cut at 125ipm, 1/2" DOC.

Share this post


Link to post
Share on other sites

I could definitely be more aggressive on cuts but I'm not cutting sheet goods and the production rate is what I choose, jobs I contract, etc. and working out of our home shop.  Most of what I cut is Walnut 0.80" thick with some Maple and Cherry thrown in from time to time.  Our machine is plenty stout and powerful enough to go much faster but I'm ok with how it's all working right now.  Having said that, though, 15 months ago when I started on the CNC the fastest I cut was about 50 ipm in the same setting.  So who knows where I'll be in 6 months... I may bump it from 125 ipm all the way to 130 ipm - LOL!  Ok, maybe 150 to 175 ipm.

The last time I surfaced the spoilboard I cut it at 400 ipm just to see what that was like and it was a hoot!

David

Share this post


Link to post
Share on other sites

Yeah, the first time I went that fast I was holding my breath the whole time while surfacing the spoilboard... Could have made a diamond with how hard I was clenching...

  • Like 1

Share this post


Link to post
Share on other sites

Several years ago we introduced a machine at IWF that we programmed to through cut 3/4" melamine coated particle board cabinet parts at 4500 ipm. That was scary.

  • Like 1

Share this post


Link to post
Share on other sites
On 2/27/2018 at 3:38 PM, Mick S said:

Several years ago we introduced a machine at IWF that we programmed to through cut 3/4" melamine coated particle board cabinet parts at 4500 ipm. That was scary.

Holy dookie.

Share this post


Link to post
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.