Topics

start-up assumptions confirmation?

John Ferguson
 

My installation is in Eagle 8.1.1 running in Ubuntu 16.04. I had some
problems with the pcbgcode menus which seem to have been driven by setup
not being able to find the *.gif files and using a default which made
the menus too long to fully access. I fixed this by hard coding the
path to each of the three gifs the setup uses,
/home/john/eagle-8.1.1/pcbgcode/docs/images/z_axis.gif for example.


I realize that this problem is likely symptomatic of a screwed up
installation, but once i did it, everything worked.


After some initial confusion in setting up design rules in Eagle, I
designed, autorouted, adjusted a couple of the traces, and cut the most
amazingly precise small board with my CNC 6040 router. There were no
slivers nor any burrs - NONE. I used a 30 degree carbide etcher running
25k rpm with 8 ipm feed rate and can't see any way the results could
have been better. This is one of the only things I've ever done in this
life that produced a good result on the first try. Thank you John Johnson.


But now I want to drill holes. I'm using .0625 single side stock and I
assume that means I should set drill depth to .0630. Is this
reasonable? I have four holes which need to be .047 but all the rest
.038. I'm going to skip the tool change, and drill all of them to .038
and then open up the four with Proxxon drill press.


It appears that the milling function does not support multiple cuts
where you remove material in .020 steps until you get to the depth you
want. So again, it looks like I set the mill depth to .0630 and use a
slow speed lest I break the tool. Does that make sense?


I suppose I could do a dxf of the milling layer and export it to
SheetCAM where I could then do vertically stepped cuts. maybe not worth
the bother although this would get me the offset.


Please let me know if you see anything goofy here.


Thanks for wading through this.


john ferguson, Delray Beach

Art Eckstein
 

John,
Congratulations on getting it setup and running. It is especially nice to have it work as needed the first time out!

A lot of people have had problems using pcb-gcode with V8.x of Eagle so maybe it is pretty well ironed out in 8.1.1.  Personally, I am still using V 6.1.0 because I am a firm believer in the "If it ain't broke, don't fix it" crowd. 

Your drilling procedure is in line with good practice and should work just fine. If your using cheap pcb stock from fleebay like I am, you might want to go a tad deeper due to board thickness variation. I use .065 stock also and the last board I did, had it set to .080" deep (I have a derlin holding fixture underneath so it is not a problem).

You are correct in the fact that milling does not allow multiple steps for depth of cut and doing either by slow feed or importing into sheetcam are good alternatives.

Looks good and again congratulations on your success.

Art
Country Bubba



At 10:19 AM 5/6/2017, you wrote:
My installation is in Eagle 8.1.1 running in Ubuntu 16.04.  I had some
problems with the pcbgcode menus which seem to have been driven by setup
not being able to find the *.gif files and using a default which made
the menus too long to fully access.  I fixed this by hard coding the
path to each of the three gifs the setup uses, 
/home/john/eagle-8.1.1/pcbgcode/docs/images/z_axis.gif for example.


I realize that this problem is likely symptomatic of a screwed up
installation, but once i did it, everything worked.


After some initial confusion in setting up design rules in Eagle, I
designed, autorouted, adjusted a couple of the traces, and cut the most
amazingly precise small board with my CNC 6040 router. There were no
slivers nor any burrs - NONE. I used a 30 degree carbide etcher running
25k rpm with 8 ipm feed rate and can't see any way the results could
have been better. This is one of the only things I've ever done in this
life that produced a good result on the first try. Thank you John Johnson.


But now I want to drill holes.  I'm using .0625 single side stock and I
assume that means I should set drill depth to .0630.  Is this
reasonable? I have four holes which need to be .047 but all the rest
.038.  I'm going to skip the tool change, and drill all of them to .038
and then open up the four with Proxxon drill press.


It appears that the milling function does not support multiple cuts
where you remove material in .020 steps until you get to the depth you
want.  So again, it looks like I set the mill depth to .0630 and use a
slow speed lest I break the tool.  Does that make sense?


I suppose I could do a dxf of the milling layer and export it to
SheetCAM where I could then do vertically stepped cuts.  maybe not worth
the bother although this would get me the offset.


Please let me know if you see anything goofy here.


Thanks for wading through this.


john ferguson,  Delray Beach



John Johnson
 

Hi John,

Glad to hear of your success!
Everything you outlined sounds good. The one thing I would change is the drill depth. Since the end of the drill is angled, drilling just over the depth of the board won’t drill the full diameter through the board.
Something like this: __\/__
I would add a little over half the drill diameter to the board’s thickness. Say, 0.038/2+0.063=0.082, so ~ 0.085 and see how that works for you. Since you have a precision drill press, using the 0.038 holes as pilots for the .047 makes perfect sense.
Not sure what you’re using for a spoil board, but I’ve found MDF works pretty well. It sounds like you’re having no issues with flatness of your pc board stock, which can cause variations in etched line width, so that’s great.
I’d like to see a picture or video of your aircraft when completed!

Happy milling!

Regards,
John

Sent with Unibox

On May 6, 2017, at 10:19 AM, john jferg977@... [pcb-gcode] wrote:

My installation is in Eagle 8.1.1 running in Ubuntu 16.04. I had some 
problems with the pcbgcode menus which seem to have been driven by setup 
not being able to find the *.gif files and using a default which made 
the menus too long to fully access. I fixed this by hard coding the 
path to each of the three gifs the setup uses, 
/home/john/eagle-8.1.1/pcbgcode/docs/images/z_axis.gif for example.

I realize that this problem is likely symptomatic of a screwed up 
installation, but once i did it, everything worked.

After some initial confusion in setting up design rules in Eagle, I 
designed, autorouted, adjusted a couple of the traces, and cut the most 
amazingly precise small board with my CNC 6040 router. There were no 
slivers nor any burrs - NONE. I used a 30 degree carbide etcher running 
25k rpm with 8 ipm feed rate and can't see any way the results could 
have been better. This is one of the only things I've ever done in this 
life that produced a good result on the first try. Thank you John Johnson.

But now I want to drill holes. I'm using .0625 single side stock and I 
assume that means I should set drill depth to .0630. Is this 
reasonable? I have four holes which need to be .047 but all the rest 
.038. I'm going to skip the tool change, and drill all of them to .038 
and then open up the four with Proxxon drill press.

It appears that the milling function does not support multiple cuts 
where you remove material in .020 steps until you get to the depth you 
want. So again, it looks like I set the mill depth to .0630 and use a 
slow speed lest I break the tool. Does that make sense?

I suppose I could do a dxf of the milling layer and export it to 
SheetCAM where I could then do vertically stepped cuts. maybe not worth 
the bother although this would get me the offset.

Please let me know if you see anything goofy here.

Thanks for wading through this.

john ferguson, Delray Beach

John Ferguson
 

Gentlemen,

Thanks for the kind words.  I made a little fixture with mdf which screws down to the 6040 table and then I drill holes in the corner of the pcb material and screw it down to the drilled and tapped holes in the mdf with 6-32 nylon cap screws.  works great and on the little boards i'm using , the screws hold the board down pretty flat.  I should add that I take a light pass with a one inch fly cutter if I have to remove and replace the fixture.  I'll post photos of all this if anyone is interested. 

I also built a vacuum table from HDPE which can handle most of the cutting envelope of the router 12x22 inches.  It holds a piece of LDF which I re-surface every now and then.  vacuum is generated by a bucket-head (el cheapo) vacuum from home depot.  makes a lot of noise - have to wear ear plugs but it works.

john


On 05/06/2017 11:05 AM, John Johnson john@... [pcb-gcode] wrote:
 

Hi John,

Glad to hear of your success!
Everything you outlined sounds good. The one thing I would change is the drill depth. Since the end of the drill is angled, drilling just over the depth of the board won’t drill the full diameter through the board.
Something like this: __\/__
I would add a little over half the drill diameter to the board’s thickness. Say, 0.038/2+0.063=0.082, so ~ 0.085 and see how that works for you. Since you have a precision drill press, using the 0.038 holes as pilots for the .047 makes perfect sense.
Not sure what you’re using for a spoil board, but I’ve found MDF works pretty well. It sounds like you’re having no issues with flatness of your pc board stock, which can cause variations in etched line width, so that’s great.
I’d like to see a picture or video of your aircraft when completed!

Happy milling!

Regards,
John

Sent with Unibox

On May 6, 2017, at 10:19 AM, john jferg977@... [pcb-gcode] wrote:

My installation is in Eagle 8.1.1 running in Ubuntu 16.04. I had some 
problems with the pcbgcode menus which seem to have been driven by setup 
not being able to find the *.gif files and using a default which made 
the menus too long to fully access. I fixed this by hard coding the 
path to each of the three gifs the setup uses, 
/home/john/eagle-8.1.1/pcbgcode/docs/images/z_axis.gif for example.

I realize that this problem is likely symptomatic of a screwed up 
installation, but once i did it, everything worked.

After some initial confusion in setting up design rules in Eagle, I 
designed, autorouted, adjusted a couple of the traces, and cut the most 
amazingly precise small board with my CNC 6040 router. There were no 
slivers nor any burrs - NONE. I used a 30 degree carbide etcher running 
25k rpm with 8 ipm feed rate and can't see any way the results could 
have been better. This is one of the only things I've ever done in this 
life that produced a good result on the first try. Thank you John Johnson.

But now I want to drill holes. I'm using .0625 single side stock and I 
assume that means I should set drill depth to .0630. Is this 
reasonable? I have four holes which need to be .047 but all the rest 
.038. I'm going to skip the tool change, and drill all of them to .038 
and then open up the four with Proxxon drill press.

It appears that the milling function does not support multiple cuts 
where you remove material in .020 steps until you get to the depth you 
want. So again, it looks like I set the mill depth to .0630 and use a 
slow speed lest I break the tool. Does that make sense?

I suppose I could do a dxf of the milling layer and export it to 
SheetCAM where I could then do vertically stepped cuts. maybe not worth 
the bother although this would get me the offset.

Please let me know if you see anything goofy here.

Thanks for wading through this.

john ferguson, Delray Beach


peterg1000
 

I'm also using a 30degree carbide tool for etching pcb's on FR4 - the feed rate I use is significantly higher than indicated in John Ferguson's post.  Currently set to 500mm/min (20"/min) with a spindle speed of 18,000rpm, results are immaculate - clean edges to all traces and smooth bottoms on the isolation cuts.

Stock flatness is assured by a home made vacuum table with MDF surface machined flat in situ - checks out on a dial indicator to better than .0005" over the whole of an 8" x 4" area.  Traces and isolation  down to 0.008" can be achieved provided router backlash is properly compensated.

Machine is a Stepcraft SC420/2 with a StoneyCNC industrial grade VFD spindle.  Control software is UCCNC with U100 parallel interface into the router.  The computer is a Dell 610 running Win XP - dont need anything more fancy than that.

Peter

Herts, UK

John Ferguson
 

It's interesting Peter,

I had inadvertantly set the feed to 20 ipm on the second board I cut, caught it after board was half done and reset to 8 ipm.  I can't see any difference so I guess there is no hazard to faster cutting speeds. 

I'm using LinuxCNC running in Ubuntu 10.04.  Few of my boards will be made more than as often as it takes to get a good one - assuming I don't continue to have the wonderful luck I've had so far.

John


On 05/06/2017 12:30 PM, petergharrison@... [pcb-gcode] wrote:
 

I'm also using a 30degree carbide tool for etching pcb's on FR4 - the feed rate I use is significantly higher than indicated in John Ferguson's post.  Currently set to 500mm/min (20"/min) with a spindle speed of 18,000rpm, results are immaculate - clean edges to all traces and smooth bottoms on the isolation cuts.

Stock flatness is assured by a home made vacuum table with MDF surface machined flat in situ - checks out on a dial indicator to better than .0005" over the whole of an 8" x 4" area.  Traces and isolation  down to 0.008" can be achieved provided router backlash is properly compensated.

Machine is a Stepcraft SC420/2 with a StoneyCNC industrial grade VFD spindle.  Control software is UCCNC with U100 parallel interface into the router.  The computer is a Dell 610 running Win XP - dont need anything more fancy than that.

Peter

Herts, UK