Tail light block-off.

Share your Shapeoko created projects!
Post Reply
TonyB
Posts: 105
Joined: Mon Apr 29, 2013 3:34 am
Location: Norwalk, Ia

Tail light block-off.

Post by TonyB » Tue Sep 03, 2013 5:15 pm

The final version will be plastic, but for now I've been testing things out with wood. Since I'm still fairly new to PyCAM, TinkerCAD, and 3D stuff in general.

Here's the 3D view in TinkerCAD:
https://tinkercad.com/embed/eJRSnSCKOTO?editbtn=1

Since I wanted a way to cut the bottom, once I was done cutting the top; I essentially just duplicated the TinkerCAD file, grabbed a rectangle, and cut the inital design.
https://tinkercad.com/embed/4Lv6VqmzK4E?editbtn=1

At that point, making an upside down file seemed like a quick solution to cutting the bottom:
https://tinkercad.com/embed/freahUDB24b?editbtn=1

Image
Image
Image
Image

This picture gives you an idea of the "before".
Image

Please ignore the dirty bike... I have been too busy to clean it! Haha
Image

I also attempted to cut this out of 1/2 inch HDPE:
https://www.inventables.com/technologie ... hdpe-sheet

I used Improbable Construct's spec:
2 flute 1/8" endmill, 40% step over, 1/16" cut depth, 27000 RPM, at a feed speed of 1200 mm with good results
Though I ran into issues and gave up for the night. Too many hours in the garage this weekend, I need to take a step back and reapproach it later this week. Essentially what I found was, his specs were dead on! The Shapeoko was trucking along (1200mm/min is pretty fast!) making pretty good chip flake.

I think my two issues were:
1. I told PyCAM to use the "ignore" option for the "Milling Style" (the three options are, 1. conventional/up, 2. climb/down, 3. ignore) during my roughing passes, I'm thinking I needed "conventional/up" because when it went one direction it left a sort of stranded piece between the passes (it happened every other pass, since the "Slice removal" path strategy goes up, then down, then up, then down, etc.; which would mean it would switch Milling Styles, when it switches directions...).

2. The feed of 1200 mm was perfect for a spindle speed of 27,000 rpm, the issue was that I couldn't figure out how to adjust the plunge. I'm guessing (not really sure!) PyCAM determines the plunge based on the Spindle Speed? When I tried to enter 27,000 rpm, it reset itself to 10,000 rpm. I need to investigate why it does this and if there's a way I can get around it (manually changing the gCode, find/replace? or modifying PyCAM?). When the gCode was having the cut run at a constant rate, the chip flake was pretty good and nothing was melting. But when it changed directions or plunged, it slowed down, which caused the bit to kind of linger in one area, which then caused melting/hardening of the plastic. As I got further and further into the material, I think this somewhat minor issue became worse and worse, which eventually caused the plastic to get so hard that the end-mill wouldn't pass through it. I even messed around afterwards seeing if I could get it to go through by turning the spindle on and pushing the machine through; it wouldn't!

If anyone has any advice on what's happening, I'd love to hear it. I'd like to stick with TinkerCAD and PyCAM, so hopefully the solution would be something tailored to that concept.

Thanks!
Tony
MegaSquirted 62mm 7m @ 20psi on 91 octane
410whp/411ftlbs

Build Thread
Image

WillAdams
Posts: 8489
Joined: Mon Apr 09, 2012 6:11 pm
Location: Pennsylvania --- south of the Turnpike, East of US-15
Contact:

Re: Tail light block-off.

Post by WillAdams » Tue Sep 03, 2013 5:42 pm

Most of the GRBL communication / control programs have an option for limiting the plunge rate, so I don't worry too much about it, just set GRBL Controller to limit it to something reasonable. (Preferences | Limit Z Rate).
Shapeoko 3XL #0006 w/Makita RT0701 Router w/0.125″ and ¼″ Elaire precision collets
Nomad 883 Pro #596 (bamboo)

TonyB
Posts: 105
Joined: Mon Apr 29, 2013 3:34 am
Location: Norwalk, Ia

Re: Tail light block-off.

Post by TonyB » Tue Sep 03, 2013 6:48 pm

WillAdams wrote:Most of the GRBL communication / control programs have an option for limiting the plunge rate, so I don't worry too much about it
Don't I want it the other way around? I think the plunge rate is too slow, not too fast. If the plastic is melting, doesn't that mean one of two speeds needs decreased?
1. Spindle speed
2. Feed or Plunge speed.

In this case, the Feed is cutting next to perfect, but the Plunge is melting. So I'd think that I either need to slow the Spindle speed when Plunging or increase the Plunge speed and leave the Spindle speed constant.

I can only manually adjust Spindle speed, so I'm trying to address #2. Is that what you meant?
WillAdams wrote:just set GRBL Controller to limit it to something reasonable. (Preferences | Limit Z Rate).
I really like the Grbl Controller, I think zapmaker has done a great job on it. But I've been having some issues that I haven't tried to confront yet, where my machine just comes to a halt all of a sudden. I'm wondering if it's because I'm on an older version (3.3.2, since I'm on OSX).

So I've been using the Universal gCode Sender in the mean time.

I also wanted to get a computer setup that would only be used for my Shapeoko. I have a Windows Laptop laying around that would be perfect. I spent some time trying to install the newest version of the Grbl Controller and getting it to connect to Arduino. I downloaded Arduino's development package and got the drivers installed (to the best of my knowledge). But I couldn't get it to connect.

The next time I do a run, I'll give Grbl Controller another shot on both Mac and Windows and post my findings from both. I had some messages that would help someone point me in the right direction, I've just been busy trying to make progress.

Thanks for the insight!
Tony
MegaSquirted 62mm 7m @ 20psi on 91 octane
410whp/411ftlbs

Build Thread
Image

WillAdams
Posts: 8489
Joined: Mon Apr 09, 2012 6:11 pm
Location: Pennsylvania --- south of the Turnpike, East of US-15
Contact:

Re: Tail light block-off.

Post by WillAdams » Tue Sep 03, 2013 7:04 pm

My apologies --- my difficulties have all been in the other direction, so I missed the melting.

Things you can do to increase your Z-speed:

- search your G-code and do a global find-replace for all F settings associated w/ the Z if you can't get the software to set it automatically
- if that's not fast enough, upgrade to an Acme axis if you haven't already

I think there's an acceleration limit one can set in GRBL --- I think it's shared between all the axes though, so ought not be an issue.

Perhaps turning off micro-stepping (or using a non-micro-stepping motor) would help, but I'm really hazy on the electronics stuff.

One other possibility is to use a lead-in/out instead of a direct plunge --- you might be able to manually code those into the G-code.

Have you looked into some sort of active cooling (ISTR mentions of even an aquarium pump blowing cool air helping).
Shapeoko 3XL #0006 w/Makita RT0701 Router w/0.125″ and ¼″ Elaire precision collets
Nomad 883 Pro #596 (bamboo)

Improbable Construct
Posts: 997
Joined: Tue Apr 10, 2012 3:21 am
Location: Fairhope, AL
Contact:

Re: Tail light block-off.

Post by Improbable Construct » Tue Sep 03, 2013 9:32 pm

TonyB wrote: I used Improbable Construct's spec:

I think my two issues were:
1. I told PyCAM to use the "ignore" option for the "Milling Style" (the three options are, 1. conventional/up, 2. climb/down, 3. ignore) during my roughing passes, I'm thinking I needed "conventional/up" because when it went one direction it left a sort of stranded piece between the passes (it happened every other pass, since the "Slice removal" path strategy goes up, then down, then up, then down, etc.; which would mean it would switch Milling Styles, when it switches directions...).
With HDPE you want to use conventional milling. It does leave a fuzzy, stringy edge when you use climb milling. I generally run 400 mm plunge but you may want to use something closer to 200.
TonyB wrote: 2. The feed of 1200 mm was perfect for a spindle speed of 27,000 rpm, the issue was that I couldn't figure out how to adjust the plunge. I'm guessing (not really sure!) PyCAM determines the plunge based on the Spindle Speed? When I tried to enter 27,000 rpm, it reset itself to 10,000 rpm. I need to investigate why it does this and if there's a way I can get around it (manually changing the gCode, find/replace? or modifying PyCAM?). When the gCode was having the cut run at a constant rate, the chip flake was pretty good and nothing was melting. But when it changed directions or plunged, it slowed down, which caused the bit to kind of linger in one area, which then caused melting/hardening of the plastic. As I got further and further into the material, I think this somewhat minor issue became worse and worse, which eventually caused the plastic to get so hard that the end-mill wouldn't pass through it. I even messed around afterwards seeing if I could get it to go through by turning the spindle on and pushing the machine through; it wouldn't!
The spindle speed should not have any effect on the g code. It is only in there to tell your controller what speed to spin the spindle if you have that capability.
Plunge rate should be in your settings somewhere.
TonyB wrote:

If anyone has any advice on what's happening, I'd love to hear it. I'd like to stick with TinkerCAD and PyCAM, so hopefully the solution would be something tailored to that concept.

Thanks!
Tony
I haven't had problems with the HDPE melting and causing hard spots but it certainly is possible.
one last thought...
Are you using a new end mill? They do wear out and unfortunately pretty quickly.
Shapeoko #Classified some of the bolts may be original parts.
Shapeoko 1 # ???? Stainless plates, still in the box.
Shapeoko 2 # 3926 not stock
Shapeoko 3 # 0003
Store:
http://ImprobableConstruct.com
Twitter:
https://twitter.com/ImprblConstruct

TonyB
Posts: 105
Joined: Mon Apr 29, 2013 3:34 am
Location: Norwalk, Ia

Re: Tail light block-off.

Post by TonyB » Tue Sep 03, 2013 10:58 pm

WillAdams wrote:My apologies --- my difficulties have all been in the other direction, so I missed the melting.
That's alright, I tend to wonder if some of what I write is confusing, lol. Sometimes I don't have a whole lot of time to reread before submitting.
WillAdams wrote:Things you can do to increase your Z-speed:

- search your G-code and do a global find-replace for all F settings associated w/ the Z if you can't get the software to set it automatically
- if that's not fast enough, upgrade to an Acme axis if you haven't already
The first one was on my mind, I'll think that over and maybe give it a try.

I bought Improbable Construct's ACME upgrade awhile back. I also swapped out my plastic spacers for metal. My Z seems to be doing pretty well when it comes to flex.
WillAdams wrote:I think there's an acceleration limit one can set in GRBL --- I think it's shared between all the axes though, so ought not be an issue.

Perhaps turning off micro-stepping (or using a non-micro-stepping motor) would help, but I'm really hazy on the electronics stuff.

One other possibility is to use a lead-in/out instead of a direct plunge --- you might be able to manually code those into the G-code.

Have you looked into some sort of active cooling (ISTR mentions of even an aquarium pump blowing cool air helping).
I'm not really sure about some of this also; they sound like some things worth considering. I don't know a whole lot about micro-stepping; I assume a 'non-micro-stepping motor' would be smoother? I would think lead-in/out would have an impact, though I'm not sure if it applies to my situation. I do have a hose ran through my drag chain and a bendable nozzle that I can point towards my bit; the thought was to add cooling for cutting aluminum. I've done some cutting where I'll push the bendable nozzle through the side of the dust shoe and just blow air on the bit (which also blows the chips away). I'll start doing this again, I think it would be helpful in both moving chips and some cooling of the end-mill/material.


Improbable Construct wrote:With HDPE you want to use conventional milling. It does leave a fuzzy, stringy edge when you use climb milling.
I started to wonder! Lol.
Improbable Construct wrote:I generally run 400 mm plunge but you may want to use something closer to 200.
I'll keep that in mind.
Improbable Construct wrote:The spindle speed should not have any effect on the g code. It is only in there to tell your controller what speed to spin the spindle if you have that capability.
Plunge rate should be in your settings somewhere.
It's gotta be in there somewhere... I'll take another look the next time I have PyCAM up. I looked around yesterday when I realized what was going on, I figured it would be right below where you input the Feed rate; but there was only the Spindle speed (which got me thinking that maybe that value played into it...).
Improbable Construct wrote:I haven't had problems with the HDPE melting and causing hard spots but it certainly is possible.
one last thought...
Are you using a new end mill? They do wear out and unfortunately pretty quickly.
My end-mill is relatively new. But now that I think about it, when the HDPE got bound up in the flutes, I used something kind of sharp to clear it and I think I may have damaged the the end-mill; I went ahead and ordered another.

I was also curious to know what you use for CAD/CAM/gCode-sender.




Thanks for the help guys!
Tony
MegaSquirted 62mm 7m @ 20psi on 91 octane
410whp/411ftlbs

Build Thread
Image

TonyB
Posts: 105
Joined: Mon Apr 29, 2013 3:34 am
Location: Norwalk, Ia

Re: Tail light block-off.

Post by TonyB » Thu Sep 05, 2013 3:55 pm

I cut a new lower bearing block last night, the design incorporated a drag knife holder. Very similar to cchristianson's, except mine is all one piece.
http://www.shapeoko.com/forum/viewtopic.php?f=30&t=1842

I was going to test cut some vinyl, but my laptop died... I wish I would have at least snapped a picture.

Here's the design:
Image
I should have made the inner hole the same diameter as the inner part of the bearing, just an fyi (I had to drill it larger).

I swapped out my 1/8th inch two flute (which I've only cut wood and one or two attempts on HDPE) for my 1/8th inch carbide three flute (which I've used a little bit on aluminum). I had to take my spindle speed down from around 27,000 rpm to around 18,000 rpm. I ran a feed of 1200 mm/min, plunge of 400 mm/min, and the clockwise motion. This chipped relatively well, but still created one big strand. If I kept the big strand from getting wrapped around the end-mill, it worked well. What I found out was, if the big strand got wrapped around the end-mill, but not in the flutes, as the plunge would get deeper, the plastic would be pushed up the end-mill. As this plastic on plastic contact took place, it too generated a ton of heat! I failed 2-3 times before figuring out what was going on (thankfully the material was only $10).

So I'm thinking I'll stick with carbide and run the slowest spindle speed possible. I can't believe how much of a pain this was. I wasted a good 1/3 of my piece of material between Monday and yesterday!

I'll take another shot at milling this tail light block off this weekend.

Thanks again for the help!
Tony
MegaSquirted 62mm 7m @ 20psi on 91 octane
410whp/411ftlbs

Build Thread
Image

Post Reply