Re: gEDA-user: General Layers questions
On Wed, Mar 16, 2011 at 02:42:26AM +0100, Stephan Boettcher wrote: IMHO, as holes are circles draw on just another layer. People were asking for slots. If they find a vendor to do them, they may just draw lines on that layer as well. Else, DRC shall flag non-circles. Each such hole layer shall have a spec (attribute) to which (copper) layers they electrically connect. There will be at least one such layer for each type of blind, burried, and through via. The GUI will happily stack vias according to the selected routing style into a composites and paste them on the layout, so for simple cases nothing changes from how we work now. Ok. So via should be a circle element on hole typed layer. That object will have some description to which layers of type cooper it belongs to. And how would you describe the cooper around via on each layer? Someone wanted different cooper size/shape on different layers. Martin Kupec ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: General Layers questions
On Tue, Mar 15, 2011 at 05:47:25PM -0600, John Doty wrote: On Mar 15, 2011, at 4:32 PM, Martin Kupec wrote: We need at least hole element. And say which layers it goes through. But that's composition, so a hole is not elementary. But it's a simple case, so it's a good place to start designing the composition language. Ok. I am a bit lost here. Can you just do some proposal how to do it? Or example how it can look like? Martin Kupec ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: General Layers questions
On Tue, Mar 15, 2011 at 06:50:01PM -0400, DJ Delorie wrote: Our current way is that copper objects have implied mask openings. I suppose we could continue that, as well as adding some paste metrics there too. This is *in addition to* a separate paste layer for user-defined paste, or for footprint-defined custom paste, of course. Right now (as looking to the core) LineType has only Clearance attribute. No Mask/Paste. Pads has in addition Mask attribute. And to be clear. There will be mask layer. So you can draw anything there and it will be masked/unmasked. But it will not be in addition to some implicit mask attributes in some objects. What I am trying to figure out is how we want to draw some additional object on that layer according to an object in some copper layer. But it seems that we don't have to. Footprints will have its own mask layer which will be drawn in our mask layer. And normal lines usualy don't have mask/paste so we don't have to worry about. Martin Kupec ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: General Layers questions
As for mask and paste layers, we may want to have a way for an object in one layer be a transformed version of another layer. Example, clearing solder mask for a line, or pad, or whatever would create a linked object in the adjacent mask layer with a growth in size of size X. Where X can be 10% or could be +10mil. Just a basic transform. On a side note, how could we make special track parameters available? Meaning differential and single ended impedance. Like drawing a uber trace that is really a matched diff pair. That is a composite trace that is drawn as a virtual trace. Steve On Wed, Mar 16, 2011 at 12:51 AM, Martin Kupec martin.ku...@kupson.cz wrote: On Tue, Mar 15, 2011 at 06:50:01PM -0400, DJ Delorie wrote: Our current way is that copper objects have implied mask openings. I suppose we could continue that, as well as adding some paste metrics there too. This is *in addition to* a separate paste layer for user-defined paste, or for footprint-defined custom paste, of course. Right now (as looking to the core) LineType has only Clearance attribute. No Mask/Paste. Pads has in addition Mask attribute. And to be clear. There will be mask layer. So you can draw anything there and it will be masked/unmasked. But it will not be in addition to some implicit mask attributes in some objects. What I am trying to figure out is how we want to draw some additional object on that layer according to an object in some copper layer. But it seems that we don't have to. Footprints will have its own mask layer which will be drawn in our mask layer. And normal lines usualy don't have mask/paste so we don't have to worry about. Martin Kupec ___ 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: General Layers questions
Looking at the layers I would like to propose that the copper layer be made not specific to copper, but a conductor. Some common alternatives are silver ink traces, embedded resistors, or even more exotics like ITO (used for touch screens). For the footprints, They should have a routing keepout, different than a placement courtyard. That is don't rout on these layers in these regions. Pins and pads should have antipads that is when the pin goes through a plane this antipad is the area in the plane that is cut out for the pad on that layer. High speed signals often have the ground plane under the pad removed to minimize the capacitance/impedance change from the pad's greater area. Steve ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: General Layers questions
Martin Kupec martin.ku...@kupson.cz writes: On Wed, Mar 16, 2011 at 02:42:26AM +0100, Stephan Boettcher wrote: IMHO, .. holes are circles draw on just another layer. People were asking for slots. If they find a vendor to do them, they may just draw lines on that layer as well. Else, DRC shall flag non-circles. Each such hole layer shall have a spec (attribute) to which (copper) layers they electrically connect. There will be at least one such layer for each type of blind, burried, and through via. The GUI will happily stack vias according to the selected routing style into a composites and paste them on the layout, so for simple cases nothing changes from how we work now. Ok. So via should be a circle element on hole typed layer. No. A Via is a composit, consisting of a circle on the hole layer, and various circles on copper layers, and circles on mask layes, and thermals. A library (routing style) Via would have top, inner, (outer?), bottom copper layers, which would be mapped to physical copper layers of the layout according to some mapping, exactly as for footprints. In addition, some projects would have their own sets of Vias in a library, where those circles are expressed explicitly for the physical hole/coper layers of that board, for burried and blind vias, or special annular ring config on certain inner layers. That library shall be linked to some Via GUI to efficiently choose from. That object will have some description to which layers of type cooper it belongs to. The hole _layer_ should have that description. The default connects to all copper. Blind and burried vias require extra hole type layers, one for each set of drill stacks. This information is needed for connectivity checks mostly. Some DRC check may verify if the drilling of the stacks is feasible. I think this is simpler and more flexible that DJs proposal: to hierachically group (copper) layers into drill stacks. That would be a John D violation, since it originates from a narrow view on how PCBs are manufactured. It in no problem to reflect such a narrow view in a DRC rule, but it is a mistake to cast it into the core data structure. A HID may present the layers in such an arangement to the user. Said HID may then proceed to add the required hole layers and Via types automatically, after the user pushed the copper layers around as required for the project. And how would you describe the cooper around via on each layer? Someone wanted different cooper size/shape on different layers. Martin Kupec -- Stephan ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: General Layers questions
On Mar 16, 2011, at 4:24 AM, Stephan Boettcher wrote: Ok. So via should be a circle element on hole typed layer. No. A Via is a composit, consisting of a circle on the hole layer, and various circles on copper layers, and circles on mask layes, and thermals. The layer concept should be physical, not a metaphysical abstraction. Objects in a layer may contain holes, but a hole layer is nonsensical, a toxic conceptual shortcut. An outline layer is similarly bad: the insulating layers may all have the same shape sometimes, but not always. Trying to model things that aren't layers as if they were layers is one common mistake in this kind of tool. Equally common is leaving out layers: the insulating layers in a PCB are just as important as the copper, and have their own properties (shape, thickness, material, etc.). They're a critical part of the layer stack. The description language needs to be able to express feature p in layer x is aligned with feature q in layer y in order to build up composites. This is the geometrically sensible way to describe the result of drilling through several layers. But the geometric description language should not be tied to any particular fabrication procedure. John Doty Noqsi Aerospace, Ltd. http://www.noqsi.com/ j...@noqsi.com ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: General Layers questions
John Doty j...@noqsi.com writes: On Mar 16, 2011, at 4:24 AM, Stephan Boettcher wrote: Ok. So via should be a circle element on hole typed layer. No. A Via is a composit, consisting of a circle on the hole layer, and various circles on copper layers, and circles on mask layes, and thermals. The layer concept should be physical, not a metaphysical abstraction. Objects in a layer may contain holes, but a hole layer is nonsensical, a toxic conceptual shortcut. An outline layer is similarly bad: the insulating layers may all have the same shape sometimes, but not always. So, a via needs a separate hole in each copper and insulating layer? And each layer needs its own discription of it's shape? Trying to model things that aren't layers as if they were layers is one common mistake in this kind of tool. Equally common is leaving out layers: the insulating layers in a PCB are just as important as the copper, and have their own properties (shape, thickness, material, etc.). They're a critical part of the layer stack. The description language needs to be able to express feature p in layer x is aligned with feature q in layer y in order to build up composites. This is the geometrically sensible way to describe the result of drilling through several layers. But the geometric description language should not be tied to any particular fabrication procedure. This is all too physikal for my taste. Why are you so attached to the concept of drilling? For the design of a layout, all that matters is that there are conductive connections between layers. For me, a layer is something that the designer puts shapes on. Shapes with atributes, if required. The semantics of these shapes on a given layer shall all be the same. Some of these are required for netlisting, some are steering the physical checkout. -- Stephan ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
gEDA-user: Wiki errors
Is this wiki entry valid with regards to the section How can I get color postscript/PNG output? http://geda.seul.org/wiki/geda:faq-gschem#how_can_i_get_black_and_white _postscript_png_output I am running 1.6.1 and cannot find the entries or lines similar to those mentioned. I don't understand the line that says change the following line in either gschem-darkbg. what does that mean? Is that a file name? I cannot find background-color in files that look similar either. Kurt References Visible links Hidden links: 1. javascript:; ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
