How to avoid premature tool failure

Hi all,

I own a desktop 6040 CNC router that is made in China. I have managed to make some good test boards I designed for evaluating the capabilities of my setup. However, I noticed that the tool I use (Stepcraft's V-Router 45°) has gone bad too early. The milling quality was OK for three really small test boards and one larger 40x50mm board (please see the attached pictures). Also, I am unable to use the classic cheap V-bits (30°/0.2mm) because I get rough edges from the first run. I was pretty sure that my cheap spindle was the main problem and I was going to buy a more powerful spindle (2.2kW 24k rpm 4 pole spindle) since I would like to try cutting aluminum in the future. But, other users state in some posts that it is possible to mill PCBs even with spindle speeds as low as 7k rpm if the feeding speed is kept really slow (I use 20mm/min).

So what you think is the problem here? The spindle and/ or something else? If the spindle is the main problem which cheap alternative would you recommend if you took into account that I would also like to mill soft metals in the future? Is the 2.2kW/24k rpm Chinese spindle OK for this purpose? Should I buy a separate 60k rpm spindle only for PCB milling?

I would appreciate any advice! Here is the current setup:

Machine:
CNC 6040 with SFU1605 ball screws.
TB6560 motor drivers
Backlash must be small as shown in the results (when the tool is new and sharp). I am waiting for a digital dial indicator to verify.

Spindle:
Cheap FitSain-ER11 Collet chuck CNC Spindle 24V 8000RPM (12-36V). Tried feeding it from 20 V up to 36V but I got the same results. In the attached pictures I use 30V (noticed less vibrations). Actual RPM has not be verified yet.

Tools used: Genuine Stepcraft's V-Router 45° (success but premature tool wear) and classic cheap V-bits 30°/0.2mm (can't mill at all).

Software and settings:
Flatcam & GRBL.
Feeding 20mm/min.
Rapid travel speed 100mm/min.
No auto leveling used until now. I manually verify the board's level before starting the milling process.
Milling depth 35 ?m.
4 passes and 40% overlap.

If you need further information/ pictures please don't hesitate to ask.

Hi,
I think you are cutting to much fibreglass and dulling the tool.

Leveling of the PCB blank IS EXTREMELY CRITICAL. Its needs to be level to within 0.05mm otherwise you will
have to command your machine to cut so deep that the tool dulls rapidly.

I use Autleveller, a software utility that probes the board then modifies the gcode to accommodate any warp, bow of the board.

On 1oz copper board the copper is 0.035mm (35um) thick. I cut 0.06mm (60um) deep, but even a small board say 50mm x 50mm
board can have 0.1mm (100um) variance across the board. Autoleveller accounts for and corrects that variation.

I use 0.5mm two flute endmills because I really like the cut quality and I get 10 hours cutting on each one, assuming I don't break them, they are
very fine and break extremely easiliy. I also use engraving bits for very fine featured boards and I swap them out after about 10 hours. So it is possible
to make tools last provided you don't cut too much fibreglass.

Spin the tools as fast as you can. I have a 24000 rpm spindle, only because I cant afford a 600000 rpm one. I cut at 400mm to 600mm/min
and plunge at half that.

Craig

I have a 3020 with the standard spindle (I understand it goes up to not-quite-10K RPM, I have never measured) and I usually cut at 100mm/min just fine, at 0.06mm depth (without auto-leveling but on a HDF board pre-leveled with the mill itself). I'm using exactly those cheap 0.2mm v-bits (30 degrees I think) and yes the result is definitely on the burry side, but I've found a quick scrub with a standard kitchen scotch-brite pad removes them like magic. I need to clean the board anyway, since I'm also using a bit of oil on the surface of the PCB while cutting - may or may not help with the actual cutting but it sure traps the dust. Granted, this is not exactly a production-scale method (for any scale at all), but I find it's quite fine for occasional PCB work. I'm considering testing a thin cylindrical endmill too simply due to the width variations inherent in v-tip tools, but I'd prefer something thinner than 0.5mm - I understand one can get even 0.2mm ones for about ten bucks; no idea of course how long they'd last, even on "occasional small simple PCB" scale...

I will add my 2 cents...

If you are feeling vibration at 8000RPM, your spindle is probably not balanced well. You may get better results if you reduce the RPM further (and lower the feedrate proportionally). It will be painfully slow, but the quality and tool life may improve.

Also check the tool runout with a dial indicator if you have one. Cheap "spindles" (which are really just motors with ER11 collets slapped on) often have problems in that department too.

Watch your cutting depth. Cutting into the fiberglass substrate too deep will dull the tool quickly. With larger boards, simply levelling the board may not be enough. You may have to use software levelling (such as Autoleveller already mentioned above) or a mechanical depth limiter.

Narrow (15 or 30-degree) V-bits are not always better. Sometimes you can get better results with wider (45 or 60-degree) bits.

Even 60-degree V-bit tips are very fragile. Watch your plunge feedrate (I usually set it at half the X/Y feedrate). Avoid straight plunges, try spiral lead-ins if your CAM software supports them.

The board on the 1st photo looks pretty good, what RPM and feedrate did you use for it?

Hi,

Quote:

---

'm considering testing a thin cylindrical endmill too simply due to the width variations inherent in v-tip tools, but I'd prefer something thinner than 0.5mm - I understand one can get even 0.2mm ones for about ten bucks; no idea of course how long they'd last, even on "occasional small simple PCB" scale...

---

0.2mm is too incredibaly fragile, you'll break them before they wear out.

With 0.5mm (also fragile) I design my boards to have minimum 0.6mm intertrack/interpin spacing which allows SMD devices down to SOIC,

https://www.ebay.com/itm/10-0-50mm-0...72.m2749.l2649

$38 for ten is or $3.80 (plus shipping) is pretty good. The same company supply smaller endmills but I suspect you'll find them too fragile.

Craig

Hi,
also to use 0.2mm tools will require a spindle with very VERY VERY low runout otherwise you'll break the tool the moment it comes
in contact with the board.

Craig

First of all I would like to thank all of you for spending your time to help me address this issue.

1) Craig I found your advice really helpful and today I tried for the first time the auto bed leveling functionality given by bCNC. The results are outstanding (see the attached pictures). Bed leveling is for sure a really important step I was missing. I have already milled one small test board with one of my cheap V-bits 30°/0.1mm (better results) and now I am milling the "larger board". I will post the results probably tomorrow.

2) Blinkenlight I used your idea with the scotch-brite and the board shown in "cheap_v_bit.jpg" looks much better. However, the quality is not good enough for what I want. Right now I am trying with the 30°/0.1mm and it works better.

3) CitizenOfDreams thank you for your reply. Unfortunately I have not received my dial indicator yet. The runout on these cheap spindles must be incredibly high. Maybe this is the reason why I noticed the worst results with the V-bit 30°/0.2mm as Craig mentioned already.

For all the boards uploaded till now I use 20mm/min feedrate and 30V (~10-12k RPM but not verified yet) to the terminals of the spindle.

Hi,
while I use 0.5mm endmills mostly, I do use engraving bits when I require finer intertrack spacings than can be achieved with an endmill.

My experience is those cheap 10-15-30 degree 0.1mm engraving tools are rubbish, the tip breaks almost instantly and the cut is rubbish.
Try 45 or 60 degree bits, say 0.2mm, they are much more robust.

I get these from the same supplier of my 0.5mm endmills. Note they are actually double the price of the endmills, but they have proven to have good cut
quality and last for 10-12 hours cutting.

https://www.ebay.com/itm/60-DEGREE-M...72.m2749.l2649

Craig

Quote:

---

Originally Posted by joeavaerage

Hi,
while I use 0.5mm endmills mostly, I do use engraving bits when I require finer intertrack spacings than can be achieved with an endmill.

My experience is those cheap 10-15-30 degree 0.1mm engraving tools are rubbish, the tip breaks almost instantly and the cut is rubbish.
Try 45 or 60 degree bits, say 0.2mm, they are much more robust.

I get these from the same supplier of my 0.5mm endmills. Note they are actually double the price of the endmills, but they have proven to have good cut
quality and last for 10-12 hours cutting.

https://www.ebay.com/itm/60-DEGREE-M...72.m2749.l2649

Craig

---

The first milling I tried was with something like this one:

https://m.aliexpress.com/item/2037306745.html?trace=wwwdetail2mobilesitedetail

I had a pretty clean cutout. For the first 15 secs... Then it just broke.
The one you mention seems really good and it looks similar to the one we use in the LPKF milling machine we have in our university. They call it micro cutter and has a variable cutting width 0.2-0.5mm. I am going to order one for 14€ but this is almost twice the price I gave for the Stepcraft's V-router with which I had these great results shown in the first picture I posted. I hope that from now on, with autolevelling step added before milling, the bit's life will substantially increase.

I will continue the tests and report the results.

Hi,

Quote:

---

I am going to order one for 14€ but this is almost twice the price I gave for the Stepcraft's V-router with which I had these great results

---

Yes they are expensive, the only reason I got them was because I was already ordering a bunch of other stuff from the same supplier and just added a few of them
to try them out. I'm impressed, but that is not to suggest that they are the only good ones out there. I suspect any decent 60 degree cutter would outperform
the cheap 30 degree ones I had been using.

Craig

Quote:

---

Originally Posted by joeavaerage

Hi,
0.2mm is too incredibaly fragile, you'll break them before they wear out.

---

Oh, I expect there might be trouble like that, but I'd still like a test. The V-bits I'm using are already 0.2mm at the tip after all and they don't break all _that_ often - and these cylindrical ones are basically V-bits too except for the absolute last half a millimeter or so: https://www.ebay.com/itm/0-2MM-Diame...torefresh=true
I mean they might still break more often, but it seems to be worth a try. Those who scorn PCB milling never fail to point out how I can order some oh-so-very-cheaply (at about $10 cost plus another $10 shipping) so if one of these lasts more than half a PCB I've already broken even.

First results with bed leveling. Here you can see a "test_board" milled with a cheap V-bit 30°/0.1mm. The spindle is running at 26V (~9000 rpm) with less vibrations. Feeding speed remains at 20mm/min. The board is actually good enough for what I want (test_board_06.jpg) but probably it is not a 0.1mm V-bit as advertised and/ or my spindle has a pretty high runout.

In the following experiments I will set the V-bit tip diameter in FlatCAM to 0.15 or 0.2 mm. Yesterday I stopped the milling process of the "larger_board" because the cutting depth was inconsistent throughout the board area. I believe that was due to the lack of decoupling capacitors in my z-probe circuit. I added 10nF and 100pF decoupling capacitors and now the auto leveling process seems more accurate. Right now I am milling the "larger board" (cheap V-bit 30°/0.1mm | 26V ~9000 rpm | Fixed auto leveling) and I will post the results later.

Blinkenlight what type of oil you use on the surface of the PCB while cutting?

Hi,
how are you holding the PCB blank down? If you use clamps or screws around the peripherary of the board
you will 'pull' a bow or warp into the board. When the tool cuts the board the board will move, negating the effort you
took to probe the blank.

Try double sided tape to hold the board down.

Craig

Quote:

---

Originally Posted by mantalos

Blinkenlight what type of oil you use on the surface of the PCB while cutting?

---

Oh, nothing special - some sort of generic, quite thin and runny "light machinery oil" or whatever it's called. The label fell off long ago...

I'm a bit puzzled by your pics though - I seem to be getting better results than that (with the method I described) on my bog-standard 3020 and bog-standard cheap Chinese 0.2mm v-bits; one of my older pics: https://www.cnczone.com/forums/attac...0&d=1484955533

Okay, these are post-scotch-brite, but still, wtf...

Quote:

---

Originally Posted by joeavaerage

Hi,
how are you holding the PCB blank down? If you use clamps or screws around the peripherary of the board
you will 'pull' a bow or warp into the board. When the tool cuts the board the board will move, negating the effort you
took to probe the blank.

Try double sided tape to hold the board down.

Craig

---

I use a hot glue gun to attach the board on a larger piece of mdf which is also glued down to the cnc bed.

Quote:

---

Originally Posted by blinkenlight

Oh, nothing special - some sort of generic, quite thin and runny "light machinery oil" or whatever it's called. The label fell off long ago...

I'm a bit puzzled by your pics though - I seem to be getting better results than that (with the method I described) on my bog-standard 3020 and bog-standard cheap Chinese 0.2mm v-bits; one of my older pics: https://www.cnczone.com/forums/attac...0&d=1484955533

Okay, these are post-scotch-brite, but still, wtf...

---

Hmm interesting... What is the trace width in your boards? I used 8 mil (up) and 10 mil (down) traces respectively.

Hi
the issue is not trace widths but rather intertrack spacings.

I commonly use 0.4mm (10 mil) as signal trace widths and have used 0.2mm (5 mil). One advantage of using two flute endmills
is the clean cut and no trace thinning with depth that happens with a V bit. Thus I can use 0.2mm quite reliably but still prefer 0.4mm
as being easier if PCB space is not constrained.

Using 0.5mm endmills however means the intertrack spacing must be at leat 0.5mm (12.7 mil), and I allow 0.6mm (15 mil)
as it allows the software to generate a tool path that passes as a minimum twice between pins/traces.

0.6mm between traces is adequate for SIOC IC's but insufficient for finer pitches like quad flat packs. Then I am constrained to
use a V bit.

Having said that I've got my procedures down pat and very seldom do I break a 0.5mm endmill and I guess now that I have the
experience to use even smaller endmills. I had and used and eventually broke 10 of 0.4mm endmills, and I have and use some
0.3mm carbide drills. The drills being longer are very VERY fragile, I don't like using them much as they break almost by looking at them.

Craig

Quote:

---

Originally Posted by mantalos

Hmm interesting... What is the trace width in your boards? I used 8 mil (up) and 10 mil (down) traces respectively.

---

The traces are 16mil (0.4mm) and the tightest inter-track clearance is 8mil (0.2mm) which means that at ideal cutting width my 0.2mm v-bit can just about pass once between tracks (can't be less, or the software freaks out not being able to pass through there and just leaves stuff connected). In real life the milled slot is wider of course due to the v-tip, making the trace narrower - it's easily visible that the slot is more than half as wide as the trace...

Quote:

---

Originally Posted by joeavaerage

I commonly use...

---

There's... something wrong with those conversions. Which numbers are the real ones?

Hi,
my apologies, my conversion to mil was incorrect.

0.2mm trace= 8mil
0.4mm =16mil
0.6mm=24mil

Quote:

---

tightest inter-track clearance is 8mil (0.2mm) which means that at ideal cutting width my 0.2mm v-bit can just about pass once between tracks (can't be less, or the software freaks out not being able to pass through there and just leaves stuff connected).

---

That is my point, its the minimum inter-track or inter-pin spacings that determine the success or otherwise of your board.
While its possible to end up with a track thinner by virtue of a V bit, it would have to be pretty poor cutting procedure to thin a track
that much that it was discontinous. On the other hand if you are not careful the it is VERY possible for two tracks to NOT be isolated.

For this reason I tend to decide right a the outset of my PCB design what my minimum inter-pin (inter-track) spacings have to be to use
the IC's I want. That will determine the tool and procedures to be followed.

If at all possible I use SOIC IC's that have 0.6mm inter-pin spacings which in turn allows me to use 0.5mm endmills for which I have
a good supply and many hundreds hours experience in their use.

Craig

Hello,

I finished milling the "larger_board". You can see the results in the attached picture.

Settings:

1) Feeding speed = 20mm/min
2) Spindle at 22V (~7333 rpm)
3) Tool: Cheap V-bit 30°/0.1mm
4) Milling depth 50 um
5) In FlatCAM I set the tool tip to 0.2mm to get good results. Probably this is needed because my tool is not actually a 0.1mm tool and/ or my spindle has a huge runout.
6) 4 passes 40% overlap
7) Auto leveling using bCNC.
8) Added some sunflower oil on the blank pcb board. This was just an experiment because I didn't have any cutting fluid and it seems that it helped!

In this board I use 10 mil tracks. The smallest isolation distance is 0.2 mm (pad to pad for the TSSOP chip).
I edited the gcode and removed 3 out of the 4 board outlines to accelerate the milling. However, I forgot to remove a gcode command for the z axis and the machine milled a huge straight line throughout the board.
Other than that, the improvement is obvious with respect to the "cheap_v_bit.jpg?" I uploaded in the first post. What is your opinion?

Yup, that looks pretty good... :) Results look quite nice for the TSSOP chip - I don't even go below SOIC typically (which I know for sure I can mill without issues) or preferably even use DIP - size tends to not matter that much for me and DIPs either let me pass a track between pins (very useful on a single-side PCB) or offer a free "via" (if I decide to bother with double-side registration).

I'm sure there's room for experiments with other milling bits or even another spindle, but it looks like you've reached what a 3020/6040 should be able to do.

Hi,
that is a marked improvement but is still pretty raggedy.

I suspect your spindle has too much runout to do a good job. I would suugest you look to improve your machine with a 24000 rpm
spindle. They (usually) have angular contact bearings and will bring the runout down to 5um or so. You don't need alot of power
for PCB's, 750W is more than enough. If you want to do wood or aluminum then consider 1.5 -2.2kW.

The Chinese made spindles are pretty good....for the money.

I use this one from Germany:

https://www.mechatron-gmbh.de/filead...08-24-ER11.pdf

Craig

Quote:

---

Originally Posted by joeavaerage

Hi,
that is a marked improvement but is still pretty raggedy.

I suspect your spindle has too much runout to do a good job. I would suugest you look to improve your machine with a 24000 rpm
spindle. They (usually) have angular contact bearings and will bring the runout down to 5um or so. You don't need alot of power
for PCB's, 750W is more than enough. If you want to do wood or aluminum then consider 1.5 -2.2kW.

The Chinese made spindles are pretty good....for the money.

I use this one from Germany:

https://www.mechatron-gmbh.de/filead...08-24-ER11.pdf

Craig

---

Craig, you are right the results were not perfect. I will consider buying a new spindle. The one you suggested seems really good but it is too expensive for me right now. Do you think this one from aliexpress would be OK for milling aluminum?

https://www.aliexpress.com/item/3280...175b2e0e5X0dtn

Today I milled another "larger board" and I think the results are much better (see the attached pictures). Here are the settings:

1) Feeding speed = 20mm/min
2) Spindle at 22V (~7333 rpm)
3) Tool: Brand new cheap V-bit 30°/0.1mm. The one used in the last board was also used for three other failed milling jobs and it seems it wasn't as sharp as a new one.
4) Milling depth 60 um
5) In FlatCAM I set the tool tip to 0.2mm to get good results. From the results in this board probably a value of 0.15mm would be better.
6) 4 passes 40% overlap
7) Auto leveling using bCNC. In this case I used a much more dense auto level grid. Auto level probe speed set to 5mm/min.
8) Sunflower oil on the blank pcb board.
9) Used a single sided blank board of better quality.

Also, I didn't have to scrub the board. Total milling time of 4 hours. The results are actually comparable (quality not speed of course) with the $20k LPKF's ProtoMat S64 that we have in our university. What do you think?

Hi,
yes that spindle has enough power to cut aluminum, but is your machine rigid enough?

Many have tried cutting aluminum and other metals only to find that their machine is not rigid enough and
therefore cant cut metals worth a damn.

Can you post your code for the test board an I'll try to cut it and post the pics.

Craig

You can try increasing the feedrate - your chip thickness is only 0.003mm now, which is probably one of the reasons for rapid tool wear. My usual parameters are around 200mm/min at 10,000RPM.

Concerning aluminium - well, there's cutting aluminium and cutting aluminium; I don't think one can do with this kind of machine anything close to what one tends to see in videoclips where aluminium is simply ripped away like it isn't even there, in seconds, by full-size machines. On the other hand, you can cut as slow and as shallow as you like, and there's nothing magical about aluminium that would prevent you cutting it slowly enough (preferably with a dedicated Alu tool though...). I've cut 1mm thick steel plate with my bog standard 3020 and spindle - granted, slowly as hell, and I broke a half a dozen bits on the first 5cm - until I remembered to use some oil and completed the remaining dozen holes with the same single bit. So, I wouldn't count on being able to do production work in metals with these mills, but that said nothing stops you from occasionally cutting fairly soft stuff if you're patient enough...

Quote:

---

Originally Posted by joeavaerage

Hi,
yes that spindle has enough power to cut aluminum, but is your machine rigid enough?

Many have tried cutting aluminum and other metals only to find that their machine is not rigid enough and
therefore cant cut metals worth a damn.

Can you post your code for the test board an I'll try to cut it and post the pics.

Craig

---

Yes find attached the gerber files.

Regarding the aluminum milling, I think my machine is rigid enough for some light milling. No heavy production of course. Future experiments will show the actual rigidity.

Quote:

---

Originally Posted by CitizenOfDreams

You can try increasing the feedrate - your chip thickness is only 0.003mm now, which is probably one of the reasons for rapid tool wear. My usual parameters are around 200mm/min at 10,000RPM.

---

Yes I will make some new tests with higher feeding speed and report the results. Till now I believe that the most important factor that caused premature tool wear was that I was cutting very deep because of the lack of the auto level procedure. Now the noise level during the milling process is much lower and I am sure this is because the machine cuts much less of the FR4 substrate.

At the beginning I was able to mill only with the Stepcraft's V-router. Now that the process is substantially improved I can test the life of a new V-router bit.

Quote:

---

Originally Posted by blinkenlight

Concerning aluminium - well, there's cutting aluminium and cutting aluminium; I don't think one can do with this kind of machine anything close to what one tends to see in videoclips where aluminium is simply ripped away like it isn't even there, in seconds, by full-size machines. On the other hand, you can cut as slow and as shallow as you like, and there's nothing magical about aluminium that would prevent you cutting it slowly enough (preferably with a dedicated Alu tool though...). I've cut 1mm thick steel plate with my bog standard 3020 and spindle - granted, slowly as hell, and I broke a half a dozen bits on the first 5cm - until I remembered to use some oil and completed the remaining dozen holes with the same single bit. So, I wouldn't count on being able to do production work in metals with these mills, but that said nothing stops you from occasionally cutting fairly soft stuff if you're patient enough...

---

I would be really happy if I could achieve something like this:
https://www.youtube.com/watch?v=uc_O_7KjwOg

I think the specs of this machine are similar to mine.

Hi,
I too used to believe that it was possible to cut any material PROVIDED I took light enough cuts.....but......you run into the problem
that if you take a really light cut you risk the tool just 'giving it a good rub' and you generate heat but no chips.

The two determinants as to how successful you'll be are spindle torque and machine rigidity.

Without sufficient torque you will stall the spindle and break the tool. There is always the temptation to run the tool fast, once you've had a tool
where the tip turned cherry red in a few seconds will disabuse you of that idea.

The next problem is rigidity. If you create Gcode to cause the tool to engage the material for a depth of cut of 0.1mm . If the machine deflects under
that pressure by 0.09 mm then the actual cut will be only 0.01mm and you are in the territory of 'giving it a good rub'.

Best advice is try it and see.

Craig

Hi,
tried cutting your test board.

Imported the Gerber into Eagle and used the Gcode generator tool with the following properties:
Tool Tip Diameter=0.1mm
Step Over= 0.05mm (50%)
Depth=0.06mm
Speed=600mm/min, plunge 300mm/min.

I used my existing engraving tool which has had about 4-5 hours cutting prior to this job, so about 1/2 worn.

It took 43 min 45 sec.

Craig

Hi,
I notice there are a couple of places where the Gerber Import has not worked well, namely around the SMD capacitor pads and notice
also a little burring at two of the corners.

The tracks/pads in the vicinity of the IC are good.

Craig

Quote:

---

Originally Posted by joeavaerage

Hi,
I notice there are a couple of places where the Gerber Import has not worked well, namely around the SMD capacitor pads and notice
also a little burring at two of the corners.

The tracks/pads in the vicinity of the IC are good.

Craig

---

Nice! Apart from these two places the PCB looks pretty good. By the way they are not capacitors but resistors at the gates of the MOSFETs. The board is a single layer stepper controller I designed to upgrade my machine. I will upload the design to github as soon as I verify it's functionality. What tool you used? The traces seem a little thinner. Maybe 50 um would be better for your machine and/ or the tip was not sharp so the 0.1mm was not valid for the CAM software.

Hi,
I think that the tip of the tool is 0.2mm, so by me nominating a tool tip diameter of only 0.1mm would confuse the Gcode generator and make narrower tracks than target.
I did that in hopes that it might resolve the issue with the Eagle Gcode generator not 'seeing' the gap between the SMD pads.

It looks however that its the Gerber import that into Eagle that is not quite right.

Ordinarily when I design in Eagle I can quite happily use 0603 and SOT223's with this tool, but for some reason the imported Gerber does not work as well.

Craig

Quote:

---

Originally Posted by mantalos

I would be really happy if I could achieve something like this

---

Oh, you can definitely do that. I do similar things with alu enclosure end-plates with no issues whatsoever. It's more about finding the right tool/speed/feed/depth combination that avoids chips sticking/galling to the tool - that can happen and it definitely is a problem when it does.

Quote:

---

Originally Posted by joeavaerage

It looks however that its the Gerber import that into Eagle that is not quite right.

---

Are you sure Eagle can handle polygon type pads? The thing is, in traditional Gerber there is no such concept as a "rotated" pad - everything is either a circle, a vertical/horizontal rectangle, or a vertical/horizontal oval (obround). As soon as a part gets rotated with ANY non-90-degree-multiple value, its pads simply can't be expressed as standard pads any more*, only as filled polygons - which is a very much "legal" Gerber thing, but only recently becoming popular which means a lot of older Gerber implementations may have undetected issues with them (if they support them at all). And I can't help but notice that only those pads have rotation on the board...

* okay, I lied - obrounds are an exception: they can be rotated without issues to any degree because they just become "tracks" with rounded caps instead of being "flashed pads". However, recently rounded rectangle pads became popular (and IPC-7351 recommended apparently) and those can DEFINITELY be only expressed as polygon fills at ANY angle, driving the need for support. But this trend is definitely not that old in the hobby world, where Kicad wasn't even capable of any non-90 rotation for a part not that long ago.

Hi,

Quote:

---

Are you sure Eagle can handle polygon type pads?

---

Yes, Eagle uses polyangonal pads, round pads and obround pads no problems and can be rotated to any given angle.

I believe the translation from Gerber to Eagle is a bit suspect, looking at Eagels rendering of the Gerber file seems to indicate that
the outermost boundary line of a feature has considerable thickness, maybe 0.1-0.2mm. It seems that the thickness of the outer line
is encroaching on the space between features. That would describe what I saw today.

As I design in Eagle and use the ULP Gcode generator I can isolation route features as fine as 0.2mm no problems.

Craig

Yes, it looks like whatever is reading the Gerber file is doing it wrong - it's "painting" region fills with the current aperture thickness (as one would do for tracks) instead of considering the contour a zero-thickness ideal geometric object. As per the UCAMCO Gerber spec rev. 2018/11, section 4.8:

Quote:

---

Outside a region statement stroking is used to convert a segment into draw or arc graphics object. Inside a region statement a segment becomes the linear or circular contour segment.

---

That distinction is clearly lost on the importer which adds the thickness of the line to the region's contour. It's a bug...

At any rate, trying to read a Gerber back into a CAD software for CAM purposes is really a bad idea anyway - That's what things like FlatCAM are for...

Hi,

Quote:

---

At any rate, trying to read a Gerber back into a CAD software for CAM purposes is really a bad idea anyway - That's what things like FlatCAM are for...

---

Its the first time I have tried importing a Gerber file and it was not 100% sucessful. Your description of what is happening to the outline of a geometric part
sounds spot on.

I do have FlatCAM but have not really experimented with it enough yet. I also have Kicad, but have not really used it yet. I'm using my machine at work so
I tend to design in Eagle because I'm so familiar with it and I can depend on the results.

Craig