Re: gEDA-user: dxf again
On Thu, Jul 15, 2010 at 11:20 PM, Bert Timmerman wrote: > > At one moment in time it did actually compile (with a lot warnings) but the > resulting files were wrong, that is, they didn't load into AutoCAD. > > I never found enough free time for this projects to finish it into a proper > working tool. > I looked at it for a while and couldn't make heads nor tails of it, so I ended up writing my own utility: http://vivara.net/software/pcbtodxf/ It's just a little command-line thing that does what I want and no more. To be clear, it is NOT a gerber->dxf tool, rather it is a pcb->dxf tool. I want to edit pcb's input format, not output format, if that makes sense. Basically I took the dxflib example program and grafted a mono-buttocked .pcb parser onto the front of it. Seems to work. Regards, Mark markra...@gmail -- Mark Rages, Engineer Midwest Telecine LLC markra...@midwesttelecine.com ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: dxf again
If you don't need the thermal pad, I've seen QFN's be ejected from the board, without much force, when the bottom pad is not soldered. Doesn't take much twisting of a board. Many data sheets tell you in the foot notes that the pad must be solder for one or more of these reasons: Thermal, Ground, Mechanical Stability. just plunk the part on the board with flux and run a solder blob around the edges. Done. Many QFNs can look like they have nice solder points on the edges, but don't actually get any real solder under the part to the pads. These projects are prone to infant mortality failures. You will love the leadless packages if you have ever bent the pins or solder-bridged a TSSOP part. I've used both. I'll take the pins. -- [1]http://blog.softwaresafety.net/ [2]http://www.designer-iii.com/ [3]http://www.wearablesmartsensors.com/ References 1. http://blog.softwaresafety.net/ 2. http://www.designer-iii.com/ 3. http://www.wearablesmartsensors.com/ ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: dxf again
Armin Faltl wrote: Use one pad for each paste spot you need, then one overall pad with the "nopaste" flag to fill in the gaps. If I understand you right, this is an alternative to the "paste board" approach above. I'll go for this and provide the footprint when I'm ready. Looks like I got the pads and paste mask right now - thermal vias still needed but it's enough for me today ;-) (btw, this piece slurps up to 2A, so the thermal stuff is probably very much needed) Thanks again, Armin ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: dxf again
On Fri, Jul 16, 2010 at 1:35 PM, Armin Faltl wrote: > First and foremost thanks a lot! > > DJ Delorie wrote: >>> >>> I somehow feared this while I wasn't sure: so it is not posible to >>> manually define the paste mask on a footprint? >>> >> >> No. What I do is use a perl script to create a "paste board" that has >> all the paste apertures as element pads, but nothing else. Then I can >> manually edit them all, and just dump a gerber for layer 1 copper as >> the paste gerber. >> >> >>> >>> I need this to create the footprint of a part with thermal central pad. >>> >> >> Use one pad for each paste spot you need, then one overall pad with >> the "nopaste" flag to fill in the gaps. >> > > If I understand you right, this is an alternative to the "paste board" > approach above. > I'll go for this and provide the footprint when I'm ready. >>> >>> Hand-soldering is a nightmare-option with 0.5mm pad-pitch ;-) >>> >> >> No it's not, I do it all the time. Even when I use a paste stencil >> and reflow, I often have to re-solder the pins for various reasons. >> Just use enough flux and a big tip and it works just fine. >> > > I've used the surface tension of the solder with relatively fine pitched > square flat packs > and "legs" with success and actual ease. The beast I'm talking about now is > this: > > http://focus.ti.com/lit/ds/symlink/bq24103.pdf > > It has the pins beneath the package. I'll extend the pads about 0.5mm > outside (longer > with traces attached) as recommended, so will this trick work again? > > Regards, Armin > Oh, those (QFN-like) packages are quite easy to hand solder, except for the thermal pad underneath. Much easier than fragile narrow-pitch TQFP and TSSOP parts. If you don't need the thermal pad, just plunk the part on the board with flux and run a solder blob around the edges. Done. To solder the pad underneath, you need a LITTLE paste under there and an oven or hot air or a via underneath to put an iron on. You will love the leadless packages if you have ever bent the pins or solder-bridged a TSSOP part. Regards, Mark markra...@gmail -- Mark Rages, Engineer Midwest Telecine LLC markra...@midwesttelecine.com ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: dxf again
First and foremost thanks a lot! DJ Delorie wrote: I somehow feared this while I wasn't sure: so it is not posible to manually define the paste mask on a footprint? No. What I do is use a perl script to create a "paste board" that has all the paste apertures as element pads, but nothing else. Then I can manually edit them all, and just dump a gerber for layer 1 copper as the paste gerber. I need this to create the footprint of a part with thermal central pad. Use one pad for each paste spot you need, then one overall pad with the "nopaste" flag to fill in the gaps. If I understand you right, this is an alternative to the "paste board" approach above. I'll go for this and provide the footprint when I'm ready. Hand-soldering is a nightmare-option with 0.5mm pad-pitch ;-) No it's not, I do it all the time. Even when I use a paste stencil and reflow, I often have to re-solder the pins for various reasons. Just use enough flux and a big tip and it works just fine. I've used the surface tension of the solder with relatively fine pitched square flat packs and "legs" with success and actual ease. The beast I'm talking about now is this: http://focus.ti.com/lit/ds/symlink/bq24103.pdf It has the pins beneath the package. I'll extend the pads about 0.5mm outside (longer with traces attached) as recommended, so will this trick work again? Regards, Armin ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: dxf again
On Jul 16, 2010, at 7:17 AM, Armin Faltl wrote: > > Dave N6NZ wrote: >> But my application is a little different. I want to get a DXF file that I >> can run through a CAM package, in particular the paste layer, which isn't a >> 'real' layer, unfortunately -- it is synthesized in the output HID as I >> understand it. > I somehow feared this while I wasn't sure: so it is not posible to manually > define the paste mask on a footprint? > If it's possible, how? > I need this to create the footprint of a part with thermal central pad. The > manufacturer recommends the mask > should cover 55-70% of the central area while near 100% of the electrical > pads are to be covered with paste. > The industry std-solution is to "grid hatch" the large continuous areas which > also helps to keep the paste in place. > Hand-soldering is a nightmare-option with 0.5mm pad-pitch ;-) > Is it possible to define an offset to the copper area per pad? pcb footprints don't directly support that kind of complex solder mask. You might be able to employ some trickery by making the large pad out of an array of smaller pads with appropriate mask definitions and all with the same pin number. Kinda clunky. -dave > > If nothing else helps, how difficult would it be, to just create an attribute > that triggers a stub that fetches > and inserts a handcrafted gerber-snippet from a file instead of running the > generator? > > Thanks in advance, Armin > > > ___ > geda-user mailing list > geda-user@moria.seul.org > http://www.seul.org/cgi-bin/mailman/listinfo/geda-user > ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: dxf again
> I somehow feared this while I wasn't sure: so it is not posible to > manually define the paste mask on a footprint? No. What I do is use a perl script to create a "paste board" that has all the paste apertures as element pads, but nothing else. Then I can manually edit them all, and just dump a gerber for layer 1 copper as the paste gerber. > I need this to create the footprint of a part with thermal central pad. Use one pad for each paste spot you need, then one overall pad with the "nopaste" flag to fill in the gaps. > Hand-soldering is a nightmare-option with 0.5mm pad-pitch ;-) No it's not, I do it all the time. Even when I use a paste stencil and reflow, I often have to re-solder the pins for various reasons. Just use enough flux and a big tip and it works just fine. > If nothing else helps, how difficult would it be, to just create an > attribute that triggers a stub that fetches and inserts a > handcrafted gerber-snippet from a file instead of running the > generator? Not that difficult, but the trick is to make it user-friendly :-) ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: dxf again
On Thu, Jul 15, 2010 at 11:20 PM, Bert Timmerman wrote: > Hi Mark, > > Indeed, I did a half baked and buggy attempt at: > > http://github.com/bert/pcb-dxf-hid.git > > Just my EUR 0.02 (as if this first attempt to code something in C is worth > half that much ;-) > > IMHO, it might be better to do the pcb2dxf stuff as a plug-in. > > At one moment in time it did actually compile (with a lot warnings) but the > resulting files were wrong, that is, they didn't load into AutoCAD. So what was the status? I got it to compile cleanly, but it didn't make an output file. The fopen() call is never executed. Also, it appears to print things to the dxf file directly, but also links dxflib. Which approach were you trying to take? I'm thinking that my use of dxf is different than everyone else's: I want to edit in a real CAD program, then import back into pcb, but everyone else seems to want to edit gerbers in 2d cad. So maybe the tool I want is different. Regards, Mark markra...@gmail -- Mark Rages, Engineer Midwest Telecine LLC markra...@midwesttelecine.com ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: dxf again
Dave N6NZ wrote: But my application is a little different. I want to get a DXF file that I can run through a CAM package, in particular the paste layer, which isn't a 'real' layer, unfortunately -- it is synthesized in the output HID as I understand it. I somehow feared this while I wasn't sure: so it is not posible to manually define the paste mask on a footprint? If it's possible, how? I need this to create the footprint of a part with thermal central pad. The manufacturer recommends the mask should cover 55-70% of the central area while near 100% of the electrical pads are to be covered with paste. The industry std-solution is to "grid hatch" the large continuous areas which also helps to keep the paste in place. Hand-soldering is a nightmare-option with 0.5mm pad-pitch ;-) Is it possible to define an offset to the copper area per pad? If nothing else helps, how difficult would it be, to just create an attribute that triggers a stub that fetches and inserts a handcrafted gerber-snippet from a file instead of running the generator? Thanks in advance, Armin ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: dxf again
Hi Mark,
> -Original Message-
> From: geda-user-boun...@moria.seul.org
> [mailto:geda-user-boun...@moria.seul.org] On Behalf Of Mark Rages
> Sent: Friday, July 16, 2010 12:21 AM
> To: gEDA user mailing list
> Subject: Re: gEDA-user: dxf again
>
> On Thu, Jul 15, 2010 at 4:46 PM, Dave N6NZ wrote:
> >
> >
> > But my application is a little different. I want to get a
> DXF file that I can run through a CAM package, in particular
> the paste layer, which isn't a 'real' layer, unfortunately --
> it is synthesized in the output HID as I understand it. And
> while preserving dimensions is useful in some situations, I
> also want to be able to do rule-based adjustments of
> dimensions. And I also want to be able to deal with a pcb
> design from any tool.
> >
> > Anyway, my last thoughts were that pcb is the wrong place
> to do what I want to do. The correct place is a gerber2dxf
> conversion tool. The new gerbv is librarized, so one could
> write a front-end to libgerbv that read gerbers via libgerbv
> and then did the massage and output function. You might
> checkout the gerbv library API, and consider if maybe that is
> a better place to accomplish your job.
> >
>
> In my Googling, I ran across an application called "pcbtodxf"
> that purports to do gerber->dxf. No idea about licensing,
> platform etc.
>
> So it turns out there is a bitrotted dxf exporter HID at
> http://github.com/bert/pcb-dxf-hid/
>
> I'm working my way through it, trying to get it to compile.
>
> It's kind of slow going, like a 5400-line C file that has
> never been compiled before. By that, I mean there are lots
> of little mistakes like this:
>
> void somefunction( char *s ) {
> if (s == "") {
> ...etc...
>
> Of course, the compiler complains to the heavens about this,
> and it's an easy fix, but it makes me less than hopeful that
> the code's gonna work.
>
> Regards,
> Mark
> markra...@gmail
> --
> Mark Rages, Engineer
> Midwest Telecine LLC
> markra...@midwesttelecine.com
>
>
Indeed, I did a half baked and buggy attempt at:
http://github.com/bert/pcb-dxf-hid.git
Just my EUR 0.02 (as if this first attempt to code something in C is worth
half that much ;-)
IMHO, it might be better to do the pcb2dxf stuff as a plug-in.
At one moment in time it did actually compile (with a lot warnings) but the
resulting files were wrong, that is, they didn't load into AutoCAD.
I never found enough free time for this projects to finish it into a proper
working tool.
Kind regards,
Bert Timmerman.
___
geda-user mailing list
geda-user@moria.seul.org
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: dxf again
On Thu, Jul 15, 2010 at 4:46 PM, Dave N6NZ wrote:
>
>
> But my application is a little different. I want to get a DXF file that I
> can run through a CAM package, in particular the paste layer, which isn't a
> 'real' layer, unfortunately -- it is synthesized in the output HID as I
> understand it. And while preserving dimensions is useful in some situations,
> I also want to be able to do rule-based adjustments of dimensions. And I
> also want to be able to deal with a pcb design from any tool.
>
> Anyway, my last thoughts were that pcb is the wrong place to do what I want
> to do. The correct place is a gerber2dxf conversion tool. The new gerbv is
> librarized, so one could write a front-end to libgerbv that read gerbers via
> libgerbv and then did the massage and output function. You might checkout
> the gerbv library API, and consider if maybe that is a better place to
> accomplish your job.
>
In my Googling, I ran across an application called "pcbtodxf" that
purports to do gerber->dxf. No idea about licensing, platform etc.
So it turns out there is a bitrotted dxf exporter HID at
http://github.com/bert/pcb-dxf-hid/
I'm working my way through it, trying to get it to compile.
It's kind of slow going, like a 5400-line C file that has never been
compiled before. By that, I mean there are lots of little mistakes
like this:
void somefunction( char *s ) {
if (s == "") {
...etc...
Of course, the compiler complains to the heavens about this, and it's
an easy fix, but it makes me less than hopeful that the code's gonna
work.
Regards,
Mark
markra...@gmail
--
Mark Rages, Engineer
Midwest Telecine LLC
markra...@midwesttelecine.com
___
geda-user mailing list
geda-user@moria.seul.org
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: dxf again
On Jul 15, 2010, at 12:40 PM, Mark Rages wrote: > Hi all, > > Having reached the limits of pcb's feeble editor, I want to take some > traces on a pcb through a pcb->???->dxf->qcad->dxf->dxftopcb->pcb > cycle. > > I had already written the dxftopcb tool. > (http://vivara.net/software/dxftopcb) when I discovered dxf2pcb > (http://archives.seul.org/geda/user/Sep-2009/msg00134.html). > > So before I start on the pcbtodxf tool, has anybody done this already? Done, no. Thought about, yes. But my application is a little different. I want to get a DXF file that I can run through a CAM package, in particular the paste layer, which isn't a 'real' layer, unfortunately -- it is synthesized in the output HID as I understand it. And while preserving dimensions is useful in some situations, I also want to be able to do rule-based adjustments of dimensions. And I also want to be able to deal with a pcb design from any tool. Anyway, my last thoughts were that pcb is the wrong place to do what I want to do. The correct place is a gerber2dxf conversion tool. The new gerbv is librarized, so one could write a front-end to libgerbv that read gerbers via libgerbv and then did the massage and output function. You might checkout the gerbv library API, and consider if maybe that is a better place to accomplish your job. -dave PS. Another application is simply creating a component for a 3D mechanical CAD package. For that, exporting an outline layer and the drills as a .dxf would be sufficient for making a component that could be slurped into SolidWorks or FreeCAD or such. Again, probably a nice application of libgerbv. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
gEDA-user: dxf again
Hi all, Having reached the limits of pcb's feeble editor, I want to take some traces on a pcb through a pcb->???->dxf->qcad->dxf->dxftopcb->pcb cycle. I had already written the dxftopcb tool. (http://vivara.net/software/dxftopcb) when I discovered dxf2pcb (http://archives.seul.org/geda/user/Sep-2009/msg00134.html). So before I start on the pcbtodxf tool, has anybody done this already? I'm not interested in the pstoedit workaround, because I'd like to preserve layers and line widths accurately. Regards, Mark markra...@gmail -- Mark Rages, Engineer Midwest Telecine LLC markra...@midwesttelecine.com ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
