Cannot Export PCB files??

[zigzag2015]

Hi,

I have for some years exported Fusion PCB files to EAGLE that I can further process it. Today I find that the option to export in an EAGLE format is no longer an option. I can export a Fusion file format but thats no good within EAGLE.

I last used this option just this morning. Whats changed?

Craig

[zigzag2015]

Hi Jorge,

'for edge connectors it can be beneficial to include the board outline features as part of the component.'

The more I think about it, I really like that idea. Then I can slide the edge connector around on the PCB  as I like while drawing the PCB but the milling required to match the eventual part placement will in effect be carried around with it and be incorporated into the BoradOutline layer as and when required.

Craig

[LMerchell_1]

Hi Jorge,

When will the Fusion to Eagle PCB export be fully functional, as polygon cut-outs are now incompatible?

Larry

[jorge_garcia]

Hi @LMerchell_1 ,

So the cutouts should be exported to EAGLE in the old way.  My comments on this thread have been specifically about updating a ULP that was originally written with EAGLE's object types in mind. Fusion has since updated those object types and that why the ULP doesn't work, however the export to EAGLE should still be fully functional.

Try it and let me know if you see  something different.

Best Regards,

[LMerchell_1]

Yes, they should be the same. That is why I resurrected this thread, as they are different. You mention above that "For the improved version in Fusion this has become 3 different objects.", was this the reason that the Export to Eagle does not work for polygon cut-outs?

Thanks,

Larry

[zigzag2015]

Hi Seth,

I have working code but need to get a consistent procedure and Fusion Contour is not helping. This is specifically about how Fusion sets the Z height.

For some years I have used PCB-Gcode and as such it does not have a stock model. The topmost surface of the board, the copper surface, was set as zero height and you would nominate a cut depth relative to that surface. Standard 1 oz.sq.yd PCB material has a copper layer 35um thick. As standard procedure I would nominate a cut depth of 60um, that is the 35um of copper plus an extra 25um down into the fiberglass core. This ensured reliable isolation where any minor unforseen vertical variation (within 25um) would not cause a failure.

Have attached a couple of pics of the board I'm working on now. See how the Top Etch I was able to set the zero height at the top of the copper and I nominated the depth of cut be the surface of the fiberglass core PLUS 0.01mm or 10um. Note that Fusion Contour has delivered the results nicely. That is to say that the TopHeight is 0mm and the BottomHeight is -0.045mm. This is ideal and replicates how PCB-Gcode works.

The second pic is the bottom side of the same board and I used the same method to generate the toolpath but note that the zero height is set at the core surface so the TopHeight is +0.035mm and the BottomHeight is -0.01mm. Despite using an identical procedure I end up with two different toolpaths.

The TopEtch toolpath ran perfectly, once processed by Autoleveller it maintained near perfect Z height throughout the board. Not so the BotEtch toolpath. In particular when I set the material in the machine the machine get touched off to the  prevailing upper most surface namely the top of the copper. Thus when the tool path runs it runs 35um too high. I can and have manually corrected this but its not ideal.

The issue appears to be when I set the origin in the first Setup. I'd like to think that the geometry of the model includes both the 35um layer of copper traces and the fibreglass core, and when I set the top corner of the board as origin it is at the same height as the topmost surface of the copper. In the case of the TopEtch toolpath that worked perfectly but not so in the BotEtch toolpath. I've been over the selection process a dozen times and cannot find a suitable procedure that gives  repeatable results.

Can you make any suggestions?. One idea I had was to in the PCB design place a pad at the intended origin of the board and set the WCS on the surface of that pad. I'd really rather not have to bother with that, but I do need absolutely repeatable results, otherwise making PCBs requires expert attention while at the machine to correct for any changes between toolpath references.

Craig

[zigzag2015]

Hi Seth,

just after posting the above I've tumbled as to why I'm having problems.

When I did the very first stock model setup, I was in viewing the top of the model and I selected the top traces and the board core as the model. Fusion the drew a stock box that included the 35um top copper layer and the 1.5mm fibreglass core, thus the stock thickness is 1.535mm.

When I did the BotEtch toolpath the stock model was carried over from the original set-up. Thus with the board viewed from the underside the surface is the fiberglass core while the bottom traces sit above that.

What I need to do is when I do the original stock model setup is include the fiberglass core plus the top AND bottom traces so the stock model is now 1.57mm thick.

As a note to Jorge, if you want to document this case as a means for others then be sure to include this wrinkle. It applies to two sided boards.

Craig

[zigzag2015]

Hi Seth,

another question that is perplexing me is the status of the Ramp at the beginning of the toolpath. Its not a fault, the toolpath still works but is contrary to my anticipation of how it works.

The first pic is of the ramp entry to the start of a cut and the second pic is the parameters that apply to the ramp. While the ramp angle is steep (42 degrees), in practice the ramp is much lower....about 5 degrees and traverses 10mm or so over the board, while the top of the ramp is only 0.25mm above the board?

I have tried angles from 1 degree through to 80 degrees and cant see any difference in the toolpath. What am I missing?

Craig

[zigzag2015]

Hi, 

a tip to anyone else 'going down this rabbit hole' make a tool file that has all the tools that you would normally use for PCBs in one place.

For instance I use 1.5mm four flute endmills to mill the periphery of my boards, but if I select the 1.5mm endmill from my ordinary tool file it calls for flood cooling and applies a cut rate more appropriate for metals. Of course you can edit those parameters but its another step in the chain, and if you forget then

coolant floods all over the place when you did not expect it or alternately the toolpath runs much slower as if it were cutting aluminum say. 

Thus what I am doing is placing all the tools that I use for PCB's into one file, all with the appropriate default settings for PCBs. Less steps to remember equals more successful toolpaths at the first attempt. 

Another question for Seth: I have two types of files for each board. The TopEtch and BottomEtch files are one type and require a specialist Mach4Post that does not generate any G2/G3 moves. The BotDrill and BotMill files are regular Fusion machining files and thus I would use my normal Mach4 post which does include G2 and G3 moves. My question is: would it be possible to have Fusion call the appropriate post based on its the filename.? 

My thought goes that all my etch files will include 'Etch' in the filename, whereas any and all mill or drill files will have 'Mill' or 'Drill' in the filename respectively. Can I code Fusion to select one or the other post on the basis of a filename?

Craig.

[zigzag2015]

Hi Seth,

yet another question.

I find myself swapping between posts and often, not always, but often the post reverts to its default settings, in particular the section dealing with 'Clearance Height' and the other to do with 'Line numbers'. The default of the former is G28....and while its not a fault I really prefer 'Clearance Height'.

I often miss that it has changed and don'y know until the toolpath runs, not ideal.

Is it possible to set the default within the post so that they reflect my standard choices. I've found the line number preference, so that's not an issue, but I cant find the code that deals with Clearance Height, or more particularly the default?

Craig

[zigzag2015]

Hi Seth, 

think I've answered my own question. I tried Find with the search term 'clearance height'. The last match, in fact the very last block of code in the whole post

was the section I required. I edited the line             value: "G28",      to       value: "Clearance Height",

I see how that works.

Craig

[zigzag2015]

Hi,

another way to do the changing Posts thing would be to have as an option to nominate the Post to be used in the setup page, like the the attached.

I imagine that would be simpler to do than deciding on a Post based on filename and yet create a simpler workflow for PCBs.

Craig

[zigzag2015]

Hi Larry,

it was your post which triggered this flurry of activity, and that activity has resulted in me finding a solution very much on the strength of Seth's contribution that means that when EAGLE 'goes away' I will be able to continue my work. The solution I have is somewhat more time consuming to formulate, but with practice and good templates not excessive, but enjoys several advantages over the pcb-gcode solution that I have used for so many years. The machining time is reduced by at least a third using Fusion Contour rather than PCB-Gcode  for instance.

Anyway the point that I'm getting at is that you are obviously exporting something from Fusion, presumably a board, into EAGLE for some reason only to find that the export does not work. Would you explain to me why you need to export a board to EAGLE.?

I certainly have done the same thing because I believed that Fusion could not offer a comparable solution, but I've been proven wrong. It may well be that with some creativity a solution for your needs could be done WITHIN Fusion and thereby avoid the need to export at all. Especially if EAGLE disappears in a years or so time, then having an alternative is going to be required.

Craig

[zigzag2015]

Hi,

I have a question for Jorge or Seth: My current design is a very thick copper layer (12 oz/sq.yd or 420um) and for these boards I use a 0.5mm two flute end mill rather than an angled engraving bit. This board is required to sustain 250V and thus I have a toolpath that has 15 roughing passes of 0.2mm. This should result in sufficient clearance between features to withstand applied voltage. The difficulty I face is that the very first pass, the outermost roughing pass is a full width, full depth slotting pass. That is to say that the tool is expected

to cut the full depth of the copper, i.e. 420um and as it is the very first pass it will perforce be the full width of the tool, namely 0.5mm. This will almost certainly overload the tool and break it. Subsequent passes step over 0.2mm and thus the cutting load is much reduced, and I have plenty of experience to suggest that 0.42mm DOC and 0.2mm step over is fine.

What I have done in the past is to take a shallower cut, say 0.2mm to 0.25mm at the first pass, and then repeat at full depth, 0.42mm, thereafter cut at full depth with a reasonable step over.

My question is 'Can I alter the cut parameters of the very first pass of a tool path?'. Either I would cut at reduced depth, and then repeat at increasing depths until full depth is attained, or maybe cut at full depth but at a much reduced feed rate, say one third to one quarter of normal feed rate until the first pass is complete and thereafter cut at full depth at the programmed step over and the programmed normal feed rate.

Craig

[seth.madore]

Currently, that would have to be a manual process. 

Once you have your selections and settings dialed in, I would duplicate the toolpath and discard the Roughing Passes. (noting what your desired number of stepovers and stepover distance is)

In Stock to Leave, set your Radial to a math equation of Stepover*Stepover distance. For example: 4 * .09  (four steps at .09 each). This will yield a toolpath like this:

From there, you can now adjust the feedrate to your desired value as well as enable Multiple Depths

 

 

[seth.madore]

After which, I would follow-up with another Contour toolpath (using Silhouette) and Roughing Passes

[zigzag2015]

Hi Seth,

yes that makes sense. I'll try it out.

I was thinking about it overnight ans was wondering if I could reverse the order of the passes. Thus the tool path closest and adjacent to the trace would cut first and then

successive roughing passes would be outside of that. Then I could do a contour tool path at part depth with NO roughing passes with appropriate parameters, and

then a second contour path but this time full depth and with as many roughing passes as required.

Your suggestion is pretty much the reverse of that idea. Effectively using 'Radial Stock To Leave' to place a contour tool path (at part depth) at the same radial location as the

first roughing pass (at full depth) of a contour tool path with N stepover roughing passes. Great solution.

Craig 

[seth.madore]

Sadly, there isn't a super easy way to go Inside > Out with 2D Contour and your current method of selecting your contours. You'd need to project a sketch, offset a set amount and then use that sketch for the Inside > Out method. Not ideal in the slightest..

[zigzag2015]

Hi Seth,

I seemed to recall seeing a checkbox in the Contour/Passes Tab 'Preserve Order'....and that what lead to to think along those lines.

In any event I think your idea will work every bit as well, I'll try it out.

As you might imagine 12 oz.per sq.yd double sided PCB material is as 'rare as rocking horses****t' and expensive when you can find it. 

I'm down to about 2.5 sq.ft left, and I cant afford to waste it with unreliable tool paths. I don't make many boards with this material,

but I must say I found PCB-Gcode to be flexible enough to handle a partial depth tool path, which made using this material feasible.

Its not a deal  breaker but to find an alternative is going to be important and maybe a deal breaker at that time when eventually EAGLE 'goes away'.

Craig

[zigzag2015]

Hi Seth,

I am trying out the strategy you have suggested, and with a few modifications it will work just fine.

I'm not understanding how the roughing passes are allocated. Firstly Fusion insists that there be at least one finishing pass, and as a matter of consistency I programmed 0.1mm step over. I allowed four roughing passes of 0.25 nominal step over, which would in an ideal world result in the outermost tool path being (4 x 0.25)+0.1=1.1mm distant from the edge of the trace. Note is the attached pic it is nothing like that. The actual distance is about 0.8mm and with the extra 0.25mm cut width being half the tool diameter results in a copper clearance of 1.05mm. I ran the tool path and measured it.

I then tried a tool path which has four finishing passes only and nominally 0.25mm step over. This would result in (4 x 0.25mm) + 0.25mm =1.25mm copper clearance. I ran this tool path and measured the result and the copper clearance is as close as I can measure exactly 1.25mm.

In order to do a one off tool path at partial depth to avoid overloading the tool in the first slotting type pass as your strategy calls for requires the the subsequent tool paths be coincident with the first tool path, and simply the calculation of the number of roughing passes times the step over plus one for the finishing pass is not accurate, and thus the first roughing pass will not be coincident with first partial depth pass. Provided you are aware that there is this discrepancy you can increase the number of roughing passes such that it is coincident with the first pass then it works fine.

Looking at the results however I find that the very much more accurate placement of a successive number of finishing passes is a better strategy, in particular you can be better assured that the first finishing pass is going to be coincident with the first partial depth pass.

Is there a reason that successive roughing passes are not in fact one step over distant from the previous one?

Craig

[zigzag2015]

Hi,

have just finished a board made by the above strategy. It has a 420um copper layer and yet it has very clearly defined features and geometry with the tool taking the merest few um of fiber glass off the core. I'm getting fours and more tool life which points to the fact that there is no excess fiber glass removal, as fiber glass is very abrasive, and two, that there is no over loading of the tool, i.e. the tool paths is well configured. With a 0.5mm two flute endmill this later consideration is important as ANY overload, no matter how brief breaks the tool.

Craig