Best router bits?

[TDA]

What feed and speed are you using?

[Drools]

here you go John, pcb-gcode settings. I edited the resulting gcode with textpad when I set the depth to .007. I'm thinking I could have used .003 as the thickness of 2oz copper is reported to be .0028 but I'm also thinking of just going back to .005 depth.

[TDA]

Thanks. I may be missing it but I don't think RPM is on that screen. What RPM are you running at?

[Drools]

I'm not sure of the exact speed of the wolfgang spindle. I think it is some where in the range of 15K~20K.

[TDA]

I would increase your feed then. That tool should be running at 34 IPM at 15k and 45 IPM at 20k. That is where we get the best cut in copperclad (55 IPM at 24k RPM). This is of course assuming your machine can run reliably at those feeds.

[Drools]

I'm not describing what I'm seeing properly, the slivers are little islands of copper between the pads that the router failed to clear because I set the stepover too large. The bit size is .005 and I set the stepover to .005. When I set the stepover to .004 the hair thin islands should clear up. Sorry for the confusion.
I will try to increase the feed rate but the edges look fine hardly no jagged edges.

[TDA]

You were quite clear in your description. I was collecting data but thought I would pass on the info.

[Drools]

Oh ok then.
I did another board last evening with slightly different settings.
Isolationefault:0.0001
Isolation:Maximun:0.03
Isolation:Step size:0.004

Etching Tool Size: 0.005
I increased the feed rate to 30.
Z down: -0.006

The board turned out very nice but it took 8 passes.
John are you sure the bit size is 0.005 inch or is that a metric measurement? It seems to me it is smaller than 0.005? I'm still learning at this game....

Thanks
Brent

[TDA]

Went back to my trace record and I think this is from the same batch you have. Let me know if the trace is different and I will pull the QC record on it.

P/N: EM2E8-0625-60V
TRACE: 17953
QC DATE: 10/22/09
DOC: .052
TIR: .00005
DIA: .00520

One other thing to keep in mind. Even if you change your step size it may not change the actual path due to the minimum step of you machine. You may want to try and calculate the minimum step of your machine. I'll see if I can find the tread on how to do it.

Edit: If you don't have the trace number send me you invoice number by PM or email and I can pull it here.

[Drools]

Hi John, I would like to see the forumla on calculating the minimum step. My machine is using 1/10 microstepping drivers, STMD http://avrstmd.com/ , the steppers are 270oz from Tormach and finally I have 1/2-10 Acme lead screws. I purchased my bits from one of your resellers so I'm sure if I can supply the data you are looking for.
I did another board last evening with settings :
Isolation: default:0.004
Isolation: Maximun:0.03
Isolation: Step size:0.004

Etching Tool Size: 0.004
Feed rate to 30.
Z down: -0.006

The board turned out great, in 8 passes.
Now if I could only get the drill files to optimize

[Jay C]

Now if I could only get the drill files to optimize

I never bothered to try and optimize the drill files with Opti. Seemed that they already were to me as each hole in a package was drilled. Plus the need to keep all of the same sized drills together ... just didn't want to risk it.

Jay

[Drools]

The current board I'm working on has upwards of 70 holes. I do not care to change bits there are only 4 holes that require a different diameter than all the rest and I do them by hand. What I'm finding is this, depending on the component packages I use I will have 6 or more drill sizes in the nc file. I really should get busy and make up all my own packages so as to minimize all the different hole/pad sizes.
When generating the gcode I just set the tool change height to .1 and the change time to .1 so there is hardly a blip when a tool change is requested, however the default gcode does not read my mind and is all over the place when drilling.