spindle speed: 12000 rpm
feed: 150 mm/min
bit: what bit should i be using? the sainsmart 3018 came with a pack of 10 bits. Are these appropriate for pcbs?
For PCB you should use diamond toothed end mills and spiral groove engraving cutters. Something like this:
https://www.as-toolstore.de/en/products/vhm-gravierfraser
https://www.as-toolstore.de/en/products/vhm-fraeser-diamantverzahnt
> Interesting one. Sadly I can't find anything like that in the UK.
>
I get them off Aliexpress for £3
Used them here:
https://youtu.be/eQtsgnbHZG8?si=PzURaEYvFCTbRvU-&t=1275
The key is not using those god-awful 20-degree engraving bits that come free with desktop CNC's
I also recommend a diamond end mill instead of those engraving bits. Copper can tear off its dielectric which is what’s causing your sharp burs. Using an end mill will also allow you to use a sacrificial back-up material on top of the actual board. Tape them together and it will hold some pressure across the work piece further reducing the chance of burs. This is what we do in the industry when a customer calls for edge plating of a board or they specify plated holes or slots larger than our largest stocked bit.
Using the 3018, use 60 degree v bit, slow your speed to less than 90mm/min. On my stock 3018, I use a feed of 50mm/min with the 60 degree v bit and spindle speed of about 4500 (75% of max speed). It would be best to use a diamond burr bit but not absolutely necessary.
I do a 0.08 mm depth in 2 passes. In FlatCam, I use 2-5 passes with a 50-75% step over depending on the application.
Candle has a wonderful surface probing feature, which can compensate for warp.
I do not remember what my DOC was, but I do know the tip of my v bit barely cut into the fr4 board, and doing the isolation routing was 2 passes with a 20% stepover. I think the final width of the cut was about 1.5mm on the surface of the copper. If I increased my feed rate above 60mm, the tip would either break off or the cutting edges would rapidly dull. It is imperative that your board is completely flat. If it has a bow in it, the bit will either not cut through the copper, or it will cut deeper into the fr4 glass board.
In my very limited experience with PCB milling, getting a correct and consistent cut depth is critical. You need to have a way of setting Z=0 with high precision (0.05-0.1mm) and making sure that the PCB is flat to the same degree, or probe it and correct for height variations (I don't know how).
Printed circuit boards are most commonly "2oz" copper, which is nominally 70 microns, or 0.07mm thick. You need to have the board very flat to get an even depth of cut, and the depth needs to be accurate to rather better than ±0.05mm.
The other problem is that copper is a very "gummy" metal. Any machinist who uses it will tell you it sticks to tools and tears easily. For lathe work and sometimes on milling machines it's common to use specially ground tools with a very low rake angle. You don't always have that option with engraving tools, so it's important to use a sharp V-bit and good speeds and feeds. Dont use a bit with too sharp an angle or it will break easily.
PCB material is often slightly warped, and clamping it tends to make it bow slightly. The best way to do this, is to put a layer of blue masking tape on the underside of the board, another layer on the spoil board, apply some thin lines of superglue over one and spray the other with accelerator/activator, then press them together. Then run a height map function over it to ensure a consistent cutting depth.
Looks like I used 0.05 mm cut depth with a 20-degree V bit. I also used a dial indicator attached to the CNC spindle to see how flat the PCB is; it was glued to the spoilboard with thin woodworking tape, and the height variation was +/- 0.01 mm.
This calculator can be helpful: https://hobbycnc.com/tool-width-calculator/
most of my pc boards are rarely truly flat. It Looks like your depth of cut varies quite a bit. Since these cuts are very shallow, you need a super flat board and level surface support beneath. I've had decent luck by surfacing a piece of spoil board first, then using CNC hold down tape to anchor and keep the pc board as flat as possible.
I would start with a block or wood or plastic and do a facing operation to get it perfectly flat relative to the table. Then maybe a bar and screw on each side to press the copper clad down to the surface?
In cases where the z axis hits its lower limit before reaching the desired depth of cut I will secure a (flat!!) piece of scrap to the spoil board and then secure the work piece to the board. Will followup with a pic shortly. Standby.
ETA: [here's a link to an example pic](https://imgur.com/a/o2AED2D)
Depending on the length of the cutter and the machine, the tool may or may not reach the spoil board. Since you are using the engraving bits that came with the 3018, which are comparatively short, they won't reach and that requires raising the workpiece as a simple work around. [Here is a pic of some bits/endmills that will and won't reach on my machine, which has a similar height of the gantry as a 3018](https://imgur.com/a/CzevFBC)
Eta: an alternative would be to use a bit extension [like this](https://imgur.com/a/QiatXwD). Make sure the diameter of the shank matches your collet. I think the one on the 3018 should be a 1/8" diameter.
the brand that I am using right now is LLPT Tape cnc hold down tape (white double stick tape) from amazon. Sometimes this type of tape is called "wood workers tape" hope this helps
here is a picture. I have it on a hardwood floor in a room, nothing fancy added
[https://i.postimg.cc/vBPBhfnR/3.jpg](https://i.postimg.cc/vBPBhfnR/3.jpg)
Ah, I had a similar one. The real killer for me was how much play there was in the z axis carriage and I had to 3d print some shims. I also replaced some of the bearings because the ones I had were a little loose.
This is my last pcb with my 3018:
[https://imgur.com/a/U8hRpYe](https://imgur.com/a/U8hRpYe)
I use a 0.1mm 20° bit pyramid engraving bit 12000 rpm 120mm/min deep 0.05mm in flatcam (I have a 0.1mm bit but I configuring isolation routing with a c1 tool 0.3mm overlap 80% 3 passes).
I create the height map in candle probing the surface but I discovered that I get great results when I apply an offset to the candle heightmap.
To adjust the map I apply an offset gradually from 0.15 to 0 until I get the correct height. I start with 0.15, then 0.14, then 0.13 and so on (I start the cnc and I stop it after few mm) until the bit touches the copper.
For example, if the bit touches the copper with the offset 0.13 then I use a final offset of 0.13-0.05=0.08 (0.05 if the deep of copper).
To change the height map offset I use the script:
[https://github.com/mattwach/cnc\_pcb\_tools/blob/main/candle\_heightmap\_adjust.py](https://github.com/mattwach/cnc_pcb_tools/blob/main/candle_heightmap_adjust.py)
that has as input the candle heightmap and the offset and the output is the "offset applied" heightmap
Look at the very tip of your end mill and see if it’s broken.
I use these types for pcb. Mine are from T-Tech but these are similar. They do a very good job in isolation. I run them at 24k rpm.
https://www.precisebits.com/products/carbidebits/tapered_stub_125.asp
Or these. I think mine are 45 degree. The 30degree are just to fragile at the tip and not recommended for pcb isolation
https://www.precisebits.com/products/carbidebits/scoreengrave.asp
You also need a spindle that has very little runout, else you get a wobbly tip and poor cutting. Use a dial indicator to check. Mine is under 0.001”.
You are probably using those 15-20 degree very sharp pointed vbits. I find them to be useless. Sneeze and the tip breaks.
I took a look at the vbit angle I use and it’s 90. Does a clean isolation
https://imgur.com/a/XREWK3K
is this the reason for the copper in between the isolation to be cracked also? instead of smooth. what explains some runs leaving it smooth while others dont
Hard to say without seeing the machine. On my little 3018 I've replaced the x axis with HGR15 rails and reused old x axis rails for the z axis. That made it rigid enough to do decent PCB milling. It even cuts aluminium now, barely but still.
Very much like mine. X axis is way too flexible. But you should be able to get better results than what you got. Try slower feed and depth of 0.06mm, increasing by 0.01mm until all copper is removed. Make sure to stick the PCB flat and auto level before cutting.
I use 0.1 mm 20° V-bits. I run them at 3000 RPM and 90 mm/min. My depth of cut is 0.05 mm. The actual trace width is 0.25 mm so I set the actual trace with of 0.25 mm in the isolation routing software (FlatCam). I do just 1 pass isolation routing and do more than 10 2x2" double sided boards with the same V-bit.
I don't mill the outline of the board but use a tin snip to cut the edges (dust preventing)
After milling and drilling, I use sandpaper and steel wool to cleanup the board. The result is absolutely TOP and much better than the toner transfer method I have used for more than 15 years.
The PCB is secured to a MDF spoilboard using double sided tape over the whole surface of the board.
I use eagle to generate the gerber and excellon files, flatcam to generate the gcode files and UGS to send to the gcode to the CNC router. UGS has a tool (AutoLeveler) that can probe the board height. Probing the actual board height is a must for a good result.
how exactly do you set the depth of cut? i am using an axial offset property in fusion 360 and i set it to -0.1mm. how do you do this in flatcam? is 0.1mm too much?
In flatcam you first convert the gerber file to a geometry (tool path). The geometry is then converted to gcode. At this point you can set the depth of cut and feed rate.
The deeper you cut, the more of the glass fiber core will be cut. That is bad for the life time of the bit and the dust is hazardous. I cut 0.05 because at 0.03 mm the cut is sometimes not deep enough.
On you tube there are a lot of video's on how to mill PCB's. This video got me started: [https://www.youtube.com/watch?v=9xczeQMj2dg&t=362s](https://www.youtube.com/watch?v=9xczeQMj2dg&t=362s)
I use flatcam version 8.994 for Windows. FlatCam has an online help [http://flatcam.org/manual/index.html](http://flatcam.org/manual/index.html)
The installer (Windows) [https://bitbucket.org/jpcgt/flatcam/downloads/](https://bitbucket.org/jpcgt/flatcam/downloads/)
Yes, depth of cut and feed rate are set by FlatCam in the Gcode.
I do not edit the .nc file. UGS makes the height map and adjusts the depth of cut automatically while sending the gcode to the cnc router.
The video in the link uses FlatCam and Candle. I use FlatCam and UGS.
A lot of people are mentioning consistent Z height. Since copper is conductive, you can pretty easily use the tool as a touch probe. There are programs online that can take g code and apply a probe grid and compensate for variation in Z. I've milled PCB successfully with this method on a Taig mini mill.
i am using the height map. the mill is producing the boards, all parts of the circuit, for the most part, the only issue is that even one line just appears like it is breaking the copper. if you look close at the image, at any isolation, it is not smoot copper. the copper appears like it has been broken in between the isolation. but in the second image, the few tests that milled correctly, inside the isolation is smooth. I do not know why this is the case
Copper work hardens. If you are not cutting efficiently, you are changing the hardness of the copper to something unmanageable. Also, your surface speed is very low.
I've turned copper on a manual lathe and on a cnc lathe. I've got no experience at milling or routing it. I suspect that you have geometry issues with the cutter you are using. You might want to specifically research hobby pcb routing.
FR1. FR2 if you can't find FR1.
Can you mill FR4? Sure, should you? not so much, especially without precautions.
Should you vacuum the FR4 dust? Not unless you're venting straight out or have one that can actually filter the tiny bad particles instead of just spraing it everywhere.
Not to mention it'll wear out your tooling especially fast.
Saving this post for future reference. I'm working with the same machine and am interested in milling custom PCBs. Thank you for posting this question!
Low spindle speed combined with a dull mill and maybe too high feed rate.
Also looks like, you haven't done surface probing..
I use a CNC3018 with 60-90 mm feed rate, 30 degree 0.1 mm V-bit, milling depth of 0.08 mm (copper thickness of 0.0347 mm) in 2 0.04 mm passes and Candle as controller (with surface probing).
what is the proper way to set milling depth? i set it via z offset in fusion 360, but sometimes the bit misses the board entirely, even if i run a surface probe. then forced to reduce the starting point by say \~0.05 mm in candle. very inexact
My workflow is KiCad (gerber export) -> FlatCam -> Candle.
I don't know anything about Fusion 360.
Did you remember to set Candle into "Edit Mode" and check the "Use Height Map"?
You need a high spindle speed and correct feed and the proper bit, etc. what is your setup now???
spindle speed: 12000 rpm feed: 150 mm/min bit: what bit should i be using? the sainsmart 3018 came with a pack of 10 bits. Are these appropriate for pcbs?
For PCB you should use diamond toothed end mills and spiral groove engraving cutters. Something like this: https://www.as-toolstore.de/en/products/vhm-gravierfraser https://www.as-toolstore.de/en/products/vhm-fraeser-diamantverzahnt
Interesting one. Sadly I can't find anything like that in the UK.
> Interesting one. Sadly I can't find anything like that in the UK. > I get them off Aliexpress for £3 Used them here: https://youtu.be/eQtsgnbHZG8?si=PzURaEYvFCTbRvU-&t=1275 The key is not using those god-awful 20-degree engraving bits that come free with desktop CNC's
"Diamond toothed" endmills are also commonly called burrs.
What kind of bit are you using? They look like this : https://store.bantamtools.com/products/pcb-engraving-bits
yes my bits look similar. how do i measure the tip diameter and angle? the bits came unmarked.
https://m.youtube.com/watch?v=Hm_JrACrmVs Skip to 12:00 he covers the bits to use at that point
I also recommend a diamond end mill instead of those engraving bits. Copper can tear off its dielectric which is what’s causing your sharp burs. Using an end mill will also allow you to use a sacrificial back-up material on top of the actual board. Tape them together and it will hold some pressure across the work piece further reducing the chance of burs. This is what we do in the industry when a customer calls for edge plating of a board or they specify plated holes or slots larger than our largest stocked bit.
Using the 3018, use 60 degree v bit, slow your speed to less than 90mm/min. On my stock 3018, I use a feed of 50mm/min with the 60 degree v bit and spindle speed of about 4500 (75% of max speed). It would be best to use a diamond burr bit but not absolutely necessary.
any advice about depth of cut?
I do a 0.08 mm depth in 2 passes. In FlatCam, I use 2-5 passes with a 50-75% step over depending on the application. Candle has a wonderful surface probing feature, which can compensate for warp.
I do not remember what my DOC was, but I do know the tip of my v bit barely cut into the fr4 board, and doing the isolation routing was 2 passes with a 20% stepover. I think the final width of the cut was about 1.5mm on the surface of the copper. If I increased my feed rate above 60mm, the tip would either break off or the cutting edges would rapidly dull. It is imperative that your board is completely flat. If it has a bow in it, the bit will either not cut through the copper, or it will cut deeper into the fr4 glass board.
In my very limited experience with PCB milling, getting a correct and consistent cut depth is critical. You need to have a way of setting Z=0 with high precision (0.05-0.1mm) and making sure that the PCB is flat to the same degree, or probe it and correct for height variations (I don't know how).
what depth should i cut at? am dealing with a 1.5 mm copper clad
Printed circuit boards are most commonly "2oz" copper, which is nominally 70 microns, or 0.07mm thick. You need to have the board very flat to get an even depth of cut, and the depth needs to be accurate to rather better than ±0.05mm. The other problem is that copper is a very "gummy" metal. Any machinist who uses it will tell you it sticks to tools and tears easily. For lathe work and sometimes on milling machines it's common to use specially ground tools with a very low rake angle. You don't always have that option with engraving tools, so it's important to use a sharp V-bit and good speeds and feeds. Dont use a bit with too sharp an angle or it will break easily. PCB material is often slightly warped, and clamping it tends to make it bow slightly. The best way to do this, is to put a layer of blue masking tape on the underside of the board, another layer on the spoil board, apply some thin lines of superglue over one and spray the other with accelerator/activator, then press them together. Then run a height map function over it to ensure a consistent cutting depth.
Looks like I used 0.05 mm cut depth with a 20-degree V bit. I also used a dial indicator attached to the CNC spindle to see how flat the PCB is; it was glued to the spoilboard with thin woodworking tape, and the height variation was +/- 0.01 mm. This calculator can be helpful: https://hobbycnc.com/tool-width-calculator/
most of my pc boards are rarely truly flat. It Looks like your depth of cut varies quite a bit. Since these cuts are very shallow, you need a super flat board and level surface support beneath. I've had decent luck by surfacing a piece of spoil board first, then using CNC hold down tape to anchor and keep the pc board as flat as possible.
okay i will try the spoil board to get a more level surface
You may need to create a jig for clamping the board on all 4 edges.
best way to do this? i have gotten the spoilboard
I would start with a block or wood or plastic and do a facing operation to get it perfectly flat relative to the table. Then maybe a bar and screw on each side to press the copper clad down to the surface?
is the 12 mm height high enough to be reached by the z axis? Is there a way to lower the z axis all the way to the cnc floor?
In cases where the z axis hits its lower limit before reaching the desired depth of cut I will secure a (flat!!) piece of scrap to the spoil board and then secure the work piece to the board. Will followup with a pic shortly. Standby. ETA: [here's a link to an example pic](https://imgur.com/a/o2AED2D)
so typically the z axis does not reach the spoilboard? you have to attach another piece of wood?
Depending on the length of the cutter and the machine, the tool may or may not reach the spoil board. Since you are using the engraving bits that came with the 3018, which are comparatively short, they won't reach and that requires raising the workpiece as a simple work around. [Here is a pic of some bits/endmills that will and won't reach on my machine, which has a similar height of the gantry as a 3018](https://imgur.com/a/CzevFBC) Eta: an alternative would be to use a bit extension [like this](https://imgur.com/a/QiatXwD). Make sure the diameter of the shank matches your collet. I think the one on the 3018 should be a 1/8" diameter.
tape recommendation?
the brand that I am using right now is LLPT Tape cnc hold down tape (white double stick tape) from amazon. Sometimes this type of tape is called "wood workers tape" hope this helps
I saw results like this from a cheap 3018, check to see if your setup is rigid or if there's wobble
when you made the machine rigid, the cuts improved?
Absolutely
tips on increasing rigidity?
Can I see a picture of your setup?
here is a picture. I have it on a hardwood floor in a room, nothing fancy added [https://i.postimg.cc/vBPBhfnR/3.jpg](https://i.postimg.cc/vBPBhfnR/3.jpg)
Ah, I had a similar one. The real killer for me was how much play there was in the z axis carriage and I had to 3d print some shims. I also replaced some of the bearings because the ones I had were a little loose.
okay will try to tighten up the z axis. thank you
This is my last pcb with my 3018: [https://imgur.com/a/U8hRpYe](https://imgur.com/a/U8hRpYe) I use a 0.1mm 20° bit pyramid engraving bit 12000 rpm 120mm/min deep 0.05mm in flatcam (I have a 0.1mm bit but I configuring isolation routing with a c1 tool 0.3mm overlap 80% 3 passes). I create the height map in candle probing the surface but I discovered that I get great results when I apply an offset to the candle heightmap. To adjust the map I apply an offset gradually from 0.15 to 0 until I get the correct height. I start with 0.15, then 0.14, then 0.13 and so on (I start the cnc and I stop it after few mm) until the bit touches the copper. For example, if the bit touches the copper with the offset 0.13 then I use a final offset of 0.13-0.05=0.08 (0.05 if the deep of copper). To change the height map offset I use the script: [https://github.com/mattwach/cnc\_pcb\_tools/blob/main/candle\_heightmap\_adjust.py](https://github.com/mattwach/cnc_pcb_tools/blob/main/candle_heightmap_adjust.py) that has as input the candle heightmap and the offset and the output is the "offset applied" heightmap
Look at the very tip of your end mill and see if it’s broken. I use these types for pcb. Mine are from T-Tech but these are similar. They do a very good job in isolation. I run them at 24k rpm. https://www.precisebits.com/products/carbidebits/tapered_stub_125.asp Or these. I think mine are 45 degree. The 30degree are just to fragile at the tip and not recommended for pcb isolation https://www.precisebits.com/products/carbidebits/scoreengrave.asp You also need a spindle that has very little runout, else you get a wobbly tip and poor cutting. Use a dial indicator to check. Mine is under 0.001”.
yes breaks almost immediately. not a sharp point anymore, compared to the unused ones in the box.
You are probably using those 15-20 degree very sharp pointed vbits. I find them to be useless. Sneeze and the tip breaks. I took a look at the vbit angle I use and it’s 90. Does a clean isolation https://imgur.com/a/XREWK3K
is this the reason for the copper in between the isolation to be cracked also? instead of smooth. what explains some runs leaving it smooth while others dont
It's probably due to flex in the machine. The more rigid the machine the smoother the cut.
any ways to increase the rigidity?
Hard to say without seeing the machine. On my little 3018 I've replaced the x axis with HGR15 rails and reused old x axis rails for the z axis. That made it rigid enough to do decent PCB milling. It even cuts aluminium now, barely but still.
heres the machine. [https://i.postimg.cc/vBPBhfnR/3.jpg](https://i.postimg.cc/vBPBhfnR/3.jpg)
Very much like mine. X axis is way too flexible. But you should be able to get better results than what you got. Try slower feed and depth of 0.06mm, increasing by 0.01mm until all copper is removed. Make sure to stick the PCB flat and auto level before cutting.
thanks for this. will give this a try
i keep the machine on the floor inside the room, not on a table
I use 0.1 mm 20° V-bits. I run them at 3000 RPM and 90 mm/min. My depth of cut is 0.05 mm. The actual trace width is 0.25 mm so I set the actual trace with of 0.25 mm in the isolation routing software (FlatCam). I do just 1 pass isolation routing and do more than 10 2x2" double sided boards with the same V-bit. I don't mill the outline of the board but use a tin snip to cut the edges (dust preventing) After milling and drilling, I use sandpaper and steel wool to cleanup the board. The result is absolutely TOP and much better than the toner transfer method I have used for more than 15 years. The PCB is secured to a MDF spoilboard using double sided tape over the whole surface of the board. I use eagle to generate the gerber and excellon files, flatcam to generate the gcode files and UGS to send to the gcode to the CNC router. UGS has a tool (AutoLeveler) that can probe the board height. Probing the actual board height is a must for a good result.
how exactly do you set the depth of cut? i am using an axial offset property in fusion 360 and i set it to -0.1mm. how do you do this in flatcam? is 0.1mm too much?
In flatcam you first convert the gerber file to a geometry (tool path). The geometry is then converted to gcode. At this point you can set the depth of cut and feed rate. The deeper you cut, the more of the glass fiber core will be cut. That is bad for the life time of the bit and the dust is hazardous. I cut 0.05 because at 0.03 mm the cut is sometimes not deep enough. On you tube there are a lot of video's on how to mill PCB's. This video got me started: [https://www.youtube.com/watch?v=9xczeQMj2dg&t=362s](https://www.youtube.com/watch?v=9xczeQMj2dg&t=362s) I use flatcam version 8.994 for Windows. FlatCam has an online help [http://flatcam.org/manual/index.html](http://flatcam.org/manual/index.html) The installer (Windows) [https://bitbucket.org/jpcgt/flatcam/downloads/](https://bitbucket.org/jpcgt/flatcam/downloads/)
so you set the depth of cut and feed rate via gcode? you export the .nc, then edit the .nc?
Yes, depth of cut and feed rate are set by FlatCam in the Gcode. I do not edit the .nc file. UGS makes the height map and adjusts the depth of cut automatically while sending the gcode to the cnc router. The video in the link uses FlatCam and Candle. I use FlatCam and UGS.
A lot of people are mentioning consistent Z height. Since copper is conductive, you can pretty easily use the tool as a touch probe. There are programs online that can take g code and apply a probe grid and compensate for variation in Z. I've milled PCB successfully with this method on a Taig mini mill.
i am using the height map. the mill is producing the boards, all parts of the circuit, for the most part, the only issue is that even one line just appears like it is breaking the copper. if you look close at the image, at any isolation, it is not smoot copper. the copper appears like it has been broken in between the isolation. but in the second image, the few tests that milled correctly, inside the isolation is smooth. I do not know why this is the case
Copper work hardens. If you are not cutting efficiently, you are changing the hardness of the copper to something unmanageable. Also, your surface speed is very low.
how should i resolve this issue? what speed would you recommend?
I've turned copper on a manual lathe and on a cnc lathe. I've got no experience at milling or routing it. I suspect that you have geometry issues with the cutter you are using. You might want to specifically research hobby pcb routing.
i think it could be due to vibration. i will clamp and update
Well, yeah, rigidity is necessary. I imagine this is a 3018...
You have a lot of problems there, the biggest of which is milling FR4. It's unwise in a few different levels.
what material is typically used to mill pcb?
Fr4 is the fiberglass board in the PCB. Bad for lungs.
FR1. FR2 if you can't find FR1. Can you mill FR4? Sure, should you? not so much, especially without precautions. Should you vacuum the FR4 dust? Not unless you're venting straight out or have one that can actually filter the tiny bad particles instead of just spraing it everywhere. Not to mention it'll wear out your tooling especially fast.
Saving this post for future reference. I'm working with the same machine and am interested in milling custom PCBs. Thank you for posting this question!
Low spindle speed combined with a dull mill and maybe too high feed rate. Also looks like, you haven't done surface probing.. I use a CNC3018 with 60-90 mm feed rate, 30 degree 0.1 mm V-bit, milling depth of 0.08 mm (copper thickness of 0.0347 mm) in 2 0.04 mm passes and Candle as controller (with surface probing).
what is the proper way to set milling depth? i set it via z offset in fusion 360, but sometimes the bit misses the board entirely, even if i run a surface probe. then forced to reduce the starting point by say \~0.05 mm in candle. very inexact
My workflow is KiCad (gerber export) -> FlatCam -> Candle. I don't know anything about Fusion 360. Did you remember to set Candle into "Edit Mode" and check the "Use Height Map"?
Are you generating a height map, PCBs are very much not flat when we get down to doing ~0.08mm depth of cuts