Author Topic: PCB-RND  (Read 16401 times)

0 Members and 1 Guest are viewing this topic.

Online tautech

  • Super Contributor
  • ***
  • Posts: 12312
  • Country: nz
    • Taupaki Technologies Ltd.
Re: PCB-RND
« Reply #25 on: January 19, 2017, 12:35:33 pm »
..[snip]..
We are trying to be more responsive and less antisocial than the gEDA mailing list. If you are interested please join us.
..[snip]..

Editing in situ exists if people don't want to use it that is fine. They can edit the footprints in their library directly. In situ edits only change the one instance and are meant for doing *very* minor *one* *off* changes. Footprints should be drafted to spec. and if deviations are made they should be well documented. That is a user issue not a problem for the layout tool. Users of PCB mainline asked for this feature and they got it, we were not going to remove it from PCB-RND. (I have only used it once.) Insitu editing only lets you change pad/hole sizes and silk screen line thickness. You can't go remaking things completely

There is no fab I have ever seen that prints silk over directly over copper. There is there for no reason to care if someone has drawn silk over copper in their footprints. They are not modifying my data. They don't have the ability to print silk over copper directly.


Yeah, sure....

Free_electron's advice is pure Gold, but you guy's don't want to listen....
Exactly.

From a recent post FE made and just to outline his small  ;) knowledge on this matter:

One of my latest is a 22 layer and has 37.000 via's, 100.000 nets and 4000 components using 3 mil track and gap. using blind and buried and laserdrilling. Another one has 200+ ampere running through it on 8 layers using 4 ounce copper on inner layers.
Avid Rabid Hobbyist & NZ Siglent Distributor
 

Offline free_electron

  • Super Contributor
  • ***
  • Posts: 6879
  • Country: us
    • SiliconValleyGarage
Re: PCB-RND
« Reply #26 on: January 19, 2017, 03:19:21 pm »
Other useful things to have :
- body check : verify no silkscreen exists underneath any bodypart of a step file touching the pcb surface. This is especially important for things like SOP , DFN and other leadless packages. The thickness of the physical ink is enough to create pillowing problems during soldering.
- automatic sliver removal. A rule is set that no solder mask structures smaller than x should exist. X is a parameter set in the pcb file. Any violating object is automatically stripped. Some fabs can make 3 mil soldermask features, some can only do 5 or 6. I can simpy set the rule and if there are slivers. (Espcially on 0.5mm pitched parts and below )  they are removed automatically.
 Sliver detection works on soldermask and silkscreens ( should be an independent rule for both )

- automatic via tenting with pullback rule. It is a bad idea to completely cover a via with soldermask s it traps moisture in the hole. The soldermask needs to be 'opened' over the hole. Even then setting the soldermask opening to the hole size is not good. It needs to be (via holesize + constant). That constant is settable through a rule. Of course, if the via is assigned as fab or assembly testpoint ( top or bottom) then that side is opened fully, the other on closed

- thermal bleed prevention. In a library part i want to be able to specify that a pad is a not only electrical but also thermal . This creates automatically a "via farm" and a lattice pastemask that avoids the via holes. Lattice spoke width , via hole is driven from a rule , or can be set per instance through a dialog.
Backside has option to enable flood th same size as oldersize, and option to create bleedstop-rings in soldermask. That will require me showing you a drawing of such structure. These things are a pain to make by hand , but can be done in code very easily. If the software can do this it solves hours of spit and polish on a design...

- thermal spoke width assignable per net / class / device / pad.
I can throw a collection of nets , or parts in a class. To this class i can apply a rule that, if the via needs thermal spokes into the plane : this is the width, and the plane cartwheel opening. No most cad tools use a uniform width setting for the spokes. That does not make sense for high power traces connecting to the planes. Even achip like the broadcomm used on the rpi has pulsed currents of several amps on several balls.. you cant do that with 4 mil spokes...

- circular thermal / power via stitching. Click on a pad and have the tool place vias around the pad , at a set distance set from the hole , with a given via to via space (driven from rules either global or class based)
Essentially the tool needs to look at the via diameter , add the offset and create an imaginary circle of that number. On the circumference of that circle it places as many vias as possible of a given size ( hole and via size ) using the hole-to-hole clearance rules. Now these cloverleafs have to be made by hand. With this thing you simply specify the objects that need this and the tool injects them ( kind of like teardropping )

You can set rules like:

If (holesize >= 1.2) and (innet [busbar,vcc,gnd,v12]) and (incomponent [c12,c4,c19,relay9]) then createcircularstitch (holesize=0.2mm , padsize = 0.5mm , offset = 2mm hole2hole = 2.1mm)

This would create a stitch only on pins of 1.2mm that belong to components c2 c4 c9 or relay9 , and are wired to any of the given nets. Other nets / pinsizes/ parts are untouched.
It would create acircle of 1.2mm + 2mm = 3.2 mm diameter , with on its circumference vias of 0.2mm holesize and 0.5mm padsize. How many ? ((3.2mm * pi) / 2.1) degrees apart.

I have a truckload of other idea's but you can start with this...

Professional Electron Wrangler.
Any comments, or points of view expressed, are my own and not endorsed , induced or compensated by my employer(s).
 
The following users thanked this post: helius

Offline ScribblesOnNapkins

  • Regular Contributor
  • *
  • Posts: 99
Re: PCB-RND
« Reply #27 on: January 20, 2017, 08:27:24 am »
"Writing About Music is Like Dancing About Architecture" - I am not trying to reject ideas only differentiate what people are describing from what we already have. If people are willing to help break down the differences more specifically by using what we have now then I can try to bump their ideas up the queue. We have a lot of stuff currently in the works already from greater file format compatibility, and more involved layer management to field solving. I can't prioritize features requested by forum members over those from users and other developers.
 

Offline free_electron

  • Super Contributor
  • ***
  • Posts: 6879
  • Country: us
    • SiliconValleyGarage
Re: PCB-RND
« Reply #28 on: January 21, 2017, 02:46:33 pm »
You have none of what i am describing. It all has to be done manually.
If writing about music is dancing about architecture then you have the equivalent of pen and paper.
Professional Electron Wrangler.
Any comments, or points of view expressed, are my own and not endorsed , induced or compensated by my employer(s).
 

Offline nctnico

  • Super Contributor
  • ***
  • Posts: 14593
  • Country: nl
    • NCT Developments
Re: PCB-RND
« Reply #29 on: January 22, 2017, 01:40:21 am »
..[snip]..
We are trying to be more responsive and less antisocial than the gEDA mailing list. If you are interested please join us.
..[snip]..

Editing in situ exists if people don't want to use it that is fine. They can edit the footprints in their library directly. In situ edits only change the one instance and are meant for doing *very* minor *one* *off* changes. Footprints should be drafted to spec. and if deviations are made they should be well documented. That is a user issue not a problem for the layout tool. Users of PCB mainline asked for this feature and they got it, we were not going to remove it from PCB-RND. (I have only used it once.) Insitu editing only lets you change pad/hole sizes and silk screen line thickness. You can't go remaking things completely

There is no fab I have ever seen that prints silk over directly over copper. There is there for no reason to care if someone has drawn silk over copper in their footprints. They are not modifying my data. They don't have the ability to print silk over copper directly.


Yeah, sure....

Free_electron's advice is pure Gold, but you guy's don't want to listen....
No, free_electron's advice is not pure gold. It is 1) aimed at doing very complicated PCBs and/or extremely high volumes and 2) some of his suggestions are already handled by any (decent) PCB manufacturer. There is a big difference between creating a board for a low to medium volume product (say up to 10000 pieces) and creating a board which needs to be reproduced a million times where spending a day on a tedious detail pays off.

Also people who design PCBs have widely varying workflows where some want a glorified MS paint and others want their CAD software to be rigid about everything. You can't really cater to both extremes at the same time.
« Last Edit: January 22, 2017, 01:44:56 am by nctnico »
There are small lies, big lies and then there is what is on the screen of your oscilloscope.
 

Offline free_electron

  • Super Contributor
  • ***
  • Posts: 6879
  • Country: us
    • SiliconValleyGarage
Re: PCB-RND
« Reply #30 on: January 22, 2017, 01:37:02 pm »
Advice is a mixture of high end and simple. Automatic sliver removel , silkscreen clipping is something that even a hobbyist needs.
There is too much time lost in applying spit and polish - post layout.

Besides that i abolutely hate the way of thinking that "it's for hobby , mspaint will do" that is just bullshit. Hobbyists are always supposed to mess around with sub-par equipment. As a hobbyist that irritates me to no end.
« Last Edit: January 22, 2017, 01:38:56 pm by free_electron »
Professional Electron Wrangler.
Any comments, or points of view expressed, are my own and not endorsed , induced or compensated by my employer(s).
 

Offline nctnico

  • Super Contributor
  • ***
  • Posts: 14593
  • Country: nl
    • NCT Developments
Re: PCB-RND
« Reply #31 on: January 22, 2017, 02:28:35 pm »
I'm not talking about hobbyists but designs for low to medium volume production and prototypes. Every PCB manufacturer which has produced my PCB designs is perfectly capable of clipping solder mask, silk screen and other stuff to their manufacturing capabilities. Why should I bother with that? I'll probably get it wrong anyway and when my design ends up in a different factory I'd have to start allover again to cater for their specifications. Bottom line: leave PCB manufacturing specific post layout stuff to the PCB manufacturer. They get paid for it and are setup to apply their process parameters to a layout with one or two mouse clicks.

The same goes for footprints. I've dealt with lots of different assemblers over the past decades and each and every one of them has a different process and some of my designs are even made by various assemblers. Still a footprint which works fine for company A can be a total nightmare for company B so sometimes a footprint really needs some tweaking but it is rare. In some cases the assemblers apply their own rules to the PCB design when it comes to paste mask openings and other things to optimise the layout for their production process. The bottom line here is (again) to leave manufacturing specific things to the people doing the manufacturing because you generally can't foresee what the exact requirements are. However it helps to figure out what kind of footprints are the most error prone and avoid those (for example the ones with multiple pads underneath) for low to medium volume products. Unfortunately the sales droids will tell you an assembler can solder any package :scared:

You also misread my MS paint remark. Some people hate PCB packages which are too restrictive and many PCBs are so simple you don't need rules for each net or groups, etc so why waste the time to set it all up? Remember that in many small companies the designer of the circuit is also the one designing the PCB or is at least looking over the shoulder of the PCB designer. A couple of years ago I had an interesting discussion with someone who developes small RF-ish circuits. He really wanted a lot of freedom to draw the RF structures without some design rule or whatever kicking in at every corner. His boards where way too simple to use a complex package and be time efficient. To get back on topic: I can understand why some people will want the ability to adjust a footprint in a design without changing the library. It is a workflow which works most efficient for them.
« Last Edit: January 22, 2017, 02:37:10 pm by nctnico »
There are small lies, big lies and then there is what is on the screen of your oscilloscope.
 

Offline free_electron

  • Super Contributor
  • ***
  • Posts: 6879
  • Country: us
    • SiliconValleyGarage
Re: PCB-RND
« Reply #32 on: January 22, 2017, 04:00:56 pm »
This idea of aviding 'difficult footprtins' for low volume is total bullshit.
If i want to use any kind of really cool component i will use it . Even in a one off build.

Why do hobbyists eed to be restricted to bc547 transistors and so style packages ?
This is hampering innovation and the hobbyist.

I a not opposed to editing a footprit in-situ. By all means go ahead. I do understand that people want these things. I use em too. But i also want to be able to run DRC when i am building a footpritn. And have table based structures and have all the other stuff i mentioned.

Again : i do not want to take away any existing functionality. Just add tools and capabilities. Everything i have suggested does not mean breaking existing things or eliminating existing way of work.
There seems to be this notion that there should be only 'one-way' to do a certain thing.
Just give me MORE ways to do a certain thing !
Professional Electron Wrangler.
Any comments, or points of view expressed, are my own and not endorsed , induced or compensated by my employer(s).
 

Offline nctnico

  • Super Contributor
  • ***
  • Posts: 14593
  • Country: nl
    • NCT Developments
Re: PCB-RND
« Reply #33 on: January 22, 2017, 11:43:45 pm »
This idea of aviding 'difficult footprtins' for low volume is total bullshit.
If i want to use any kind of really cool component i will use it . Even in a one off build.
But be prepared to pay through the nose for the PCB and have a double digit failure rates in production! I've seen it happen a few times already. At one time I had a SoC based project where the QFN version of the power management chip was hard to get. The fine pitch BGA version however was available in large quantities but that needed (IIRC) 60um traces with 40um clearance. The customer asked me to adapt the PCB layout for the fine pitch BGA chip but they soon found out that having the PCB made wasn't economic for the volumes they wanted. In some cases you just have to be realistic about the manufacturability and accept you can't use every component out there.
There are small lies, big lies and then there is what is on the screen of your oscilloscope.
 

Offline VinzC

  • Regular Contributor
  • *
  • Posts: 171
  • Country: be
  • See you later, oscillator.
Re: PCB-RND
« Reply #34 on: February 10, 2017, 08:40:28 pm »
Quote
you guy's don't want to listen
:palm:

I'd just like to remind pcb_rnd and the project it was forked from are *both* software, which you download for free, designed by voluntaries and benevolent people. There's nothing as easy as "suggesting features"... until one has to code them. Please allow Rome to be built in more than one week if you keep that in mind.
 
The following users thanked this post: Vasi

Offline mangodan

  • Newbie
  • Posts: 1
  • Country: gb
Re: PCB-RND
« Reply #35 on: April 05, 2017, 03:08:43 am »
Hiya.  Been using geda/pcb for many years - both hobby and professional.  Just discovered this so will be sure to give it  a whirl on my next project.  unfortunately found this just after sending a couple of designs off for fab.
 

Offline grumpydoc

  • Super Contributor
  • ***
  • Posts: 2649
  • Country: gb
Re: PCB-RND
« Reply #36 on: April 09, 2017, 12:26:19 am »
Some observations as an almost complete neophyte to any EDA tool:

On my machine from a fresh install/cold start it comes up with the whole app occupying about a 16th of the screen and with the PCB area about an inch square - it's not immediately obvious what to do next.

u and R for undo & Redo, surely, world+dog (just about) uses ctrl-Z for undo and ctrl-Y for redo. There's nothing inherently better about either that pair or u/R but why swim against the tide?

Similarly z/Z for zoom rather than +/- (or ctrl + & ctrl -)

Also, as with the original I note that invoking rubber band moves with "all direction lines" not ticked is broken - it just moves the lines regardless leaving non orthogonal lines after the move. I spent some time hacking the original PCB to fix this - I'll see if I can dig out he code.
 

Offline ehughes

  • Frequent Contributor
  • **
  • Posts: 302
  • Country: us
Re: PCB-RND
« Reply #37 on: April 16, 2017, 03:10:12 pm »
I like the general direction of the parametric footprints.

One thing i have been looking for in any PCB tool is the ability to drive the entire design parametrically.   I.e.   the coordinate of a part is the coordinate of some other part plus some variable.



 

Offline VinzC

  • Regular Contributor
  • *
  • Posts: 171
  • Country: be
  • See you later, oscillator.
Re: PCB-RND
« Reply #38 on: May 12, 2017, 09:13:55 pm »
I have just tried version 1.2.2 and I like it very much as it looks already. The only thing I've noticed on the GUI side is the lack of tooltips when hovering toolbar buttons — which come from the side toolbox in the "original" pcb application. Is there a problem on my side or is it expected?
 

Offline ScribblesOnNapkins

  • Regular Contributor
  • *
  • Posts: 99
Re: PCB-RND
« Reply #39 on: June 04, 2017, 01:21:58 am »
Some observations as an almost complete neophyte to any EDA tool:

On my machine from a fresh install/cold start it comes up with the whole app occupying about a 16th of the screen and with the PCB area about an inch square - it's not immediately obvious what to do next.

u and R for undo & Redo, surely, world+dog (just about) uses ctrl-Z for undo and ctrl-Y for redo. There's nothing inherently better about either that pair or u/R but why swim against the tide?

Similarly z/Z for zoom rather than +/- (or ctrl + & ctrl -)

Also, as with the original I note that invoking rubber band moves with "all direction lines" not ticked is broken - it just moves the lines regardless leaving non orthogonal lines after the move. I spent some time hacking the original PCB to fix this - I'll see if I can dig out he code.

The key bindings are configurable in the menu file. What you get by default are the ~2 decade old key key bindings, but you are free to change any menu or key binding in the menu file.

Some users want their window manager to take care of the default size and would hate if the app wanted to remember some size, others want the app to remember window sizes and placement. We have support to both, and again this just the default. It is configurable in the preferences.

Window size is like keyboard layout if we change defaults, we may favor new users, but we piss off old users, so there's no good solution here, or at least no better solution than having it configurable, which we already have.

Sorry I did not reply faster. The code for rubber band mode is evolving now. There is a new additional rubber band mode that preserves trace angle and another mode that is targeting microwave layout. More on that in another post on our latest release.
 

Offline ScribblesOnNapkins

  • Regular Contributor
  • *
  • Posts: 99
Re: PCB-RND
« Reply #40 on: June 04, 2017, 01:25:57 am »
I like the general direction of the parametric footprints.

One thing i have been looking for in any PCB tool is the ability to drive the entire design parametrically.   I.e.   the coordinate of a part is the coordinate of some other part plus some variable.

I have been curious about that too and we are looking at some aspects of it. For it to really work though we would need more expressive metadata from the schematic capture software than just a netlist. I advocated for that on gEDA's side a long time ago. I don't think we will ever get to a totally parametrically generated layout but it would make partially autorouting layouts more attractive.
 

Offline ScribblesOnNapkins

  • Regular Contributor
  • *
  • Posts: 99
Re: PCB-RND
« Reply #41 on: June 04, 2017, 01:31:48 am »
I have just tried version 1.2.2 and I like it very much as it looks already. The only thing I've noticed on the GUI side is the lack of tooltips when hovering toolbar buttons — which come from the side toolbox in the "original" pcb application. Is there a problem on my side or is it expected?

This wasn't a priority for us compared to say updating the manual but you clearly tried the software so our lead developer dropped what he was doing and added some tooltips. It wasn't just you we did not have them. Thanks for the suggestion, people will want the tooltips at least until we get the manual sorted out!

Sadly your feature did not make our latest release but it will be in the next one. Currently if you grab the SVN head it should work.
 

Offline grumpydoc

  • Super Contributor
  • ***
  • Posts: 2649
  • Country: gb
Re: PCB-RND
« Reply #42 on: June 04, 2017, 02:42:01 am »
Some observations as an almost complete neophyte to any EDA tool:

On my machine from a fresh install/cold start it comes up with the whole app occupying about a 16th of the screen and with the PCB area about an inch square - it's not immediately obvious what to do next.

u and R for undo & Redo, surely, world+dog (just about) uses ctrl-Z for undo and ctrl-Y for redo. There's nothing inherently better about either that pair or u/R but why swim against the tide?

Similarly z/Z for zoom rather than +/- (or ctrl + & ctrl -)

Also, as with the original I note that invoking rubber band moves with "all direction lines" not ticked is broken - it just moves the lines regardless leaving non orthogonal lines after the move. I spent some time hacking the original PCB to fix this - I'll see if I can dig out he code.

The key bindings are configurable in the menu file. What you get by default are the ~2 decade old key key bindings, but you are free to change any menu or key binding in the menu file.

Some users want their window manager to take care of the default size and would hate if the app wanted to remember some size, others want the app to remember window sizes and placement. We have support to both, and again this just the default. It is configurable in the preferences.

Window size is like keyboard layout if we change defaults, we may favor new users, but we piss off old users, so there's no good solution here, or at least no better solution than having it configurable, which we already have.

Sorry I did not reply faster. The code for rubber band mode is evolving now. There is a new additional rubber band mode that preserves trace angle and another mode that is targeting microwave layout. More on that in another post on our latest release.
I appreciate that it can be hell supporting multiple environments and existing users can get very tetchy when you change the UI on them but sensible defaults for new users are not a bad thing. Apparently nothing I do makes it want to start up at a sensible size and zoom.

User configurations of basic controls is a pain - you end up with no one being able to use your set up and you not being able to use anyone else's (BTDT, got the t-shirt).

Yes, I saw that some work had been done on rubber band mode (and also that the code has changed too much for me to trivially port the work I did to the old program for this). I didn't see why it only worked on line segments which are connected to two others (is that still the case?).
 

Offline ScribblesOnNapkins

  • Regular Contributor
  • *
  • Posts: 99
Re: PCB-RND
« Reply #43 on: June 04, 2017, 12:19:49 pm »
Some observations as an almost complete neophyte to any EDA tool:

On my machine from a fresh install/cold start it comes up with the whole app occupying about a 16th of the screen and with the PCB area about an inch square - it's not immediately obvious what to do next.

u and R for undo & Redo, surely, world+dog (just about) uses ctrl-Z for undo and ctrl-Y for redo. There's nothing inherently better about either that pair or u/R but why swim against the tide?

Similarly z/Z for zoom rather than +/- (or ctrl + & ctrl -)

Also, as with the original I note that invoking rubber band moves with "all direction lines" not ticked is broken - it just moves the lines regardless leaving non orthogonal lines after the move. I spent some time hacking the original PCB to fix this - I'll see if I can dig out he code.

The key bindings are configurable in the menu file. What you get by default are the ~2 decade old key key bindings, but you are free to change any menu or key binding in the menu file.

Some users want their window manager to take care of the default size and would hate if the app wanted to remember some size, others want the app to remember window sizes and placement. We have support to both, and again this just the default. It is configurable in the preferences.

Window size is like keyboard layout if we change defaults, we may favor new users, but we piss off old users, so there's no good solution here, or at least no better solution than having it configurable, which we already have.

Sorry I did not reply faster. The code for rubber band mode is evolving now. There is a new additional rubber band mode that preserves trace angle and another mode that is targeting microwave layout. More on that in another post on our latest release.
I appreciate that it can be hell supporting multiple environments and existing users can get very tetchy when you change the UI on them but sensible defaults for new users are not a bad thing. Apparently nothing I do makes it want to start up at a sensible size and zoom.

User configurations of basic controls is a pain - you end up with no one being able to use your set up and you not being able to use anyone else's (BTDT, got the t-shirt).

Yes, I saw that some work had been done on rubber band mode (and also that the code has changed too much for me to trivially port the work I did to the old program for this). I didn't see why it only worked on line segments which are connected to two others (is that still the case?).

You should look at these.
https://archive.org/details/middle-rubber
This is the microwave thing i was talking about.
https://archive.org/details/route-radius
 

Offline grumpydoc

  • Super Contributor
  • ***
  • Posts: 2649
  • Country: gb
Re: PCB-RND
« Reply #44 on: June 04, 2017, 07:32:17 pm »
You should look at these.
https://archive.org/details/middle-rubber
This is the microwave thing i was talking about.
https://archive.org/details/route-radius
I played with the rubber band changes, haven't see the radius stuff (but had planned on adding something similar myself, just never got to it).

When I looked at it, the line segment you were moving had to be between two others - I can't see the reason for that (when I implemented it I did not have this restriction, you could move the last or first segment and it adjusted the intersection point as necessary).
 

Offline ScribblesOnNapkins

  • Regular Contributor
  • *
  • Posts: 99
Re: PCB-RND
« Reply #45 on: June 06, 2017, 01:44:59 am »
You should look at these.
https://archive.org/details/middle-rubber
This is the microwave thing i was talking about.
https://archive.org/details/route-radius
I played with the rubber band changes, haven't see the radius stuff (but had planned on adding something similar myself, just never got to it).

When I looked at it, the line segment you were moving had to be between two others - I can't see the reason for that (when I implemented it I did not have this restriction, you could move the last or first segment and it adjusted the intersection point as necessary).

The demo video doesn't show it but that works as well. It was the middle use case that was harder to code and so people wanted to show it off more.
 

Offline ScribblesOnNapkins

  • Regular Contributor
  • *
  • Posts: 99
Re: PCB-RND
« Reply #46 on: August 15, 2017, 01:19:10 am »
I started a fresh thread about the new release.
 

Offline Cerebus

  • Super Contributor
  • ***
  • Posts: 2868
  • Country: gb
Re: PCB-RND
« Reply #47 on: August 15, 2017, 03:47:57 am »
I started a fresh thread about the new release.

In some respects that might have been a bad idea. The way that the forum software works there is no universal way to 'subscribe' to or 'follow' a thread without commenting; this results in a lot of 'me too' comments in threads as the only universally effective way of following that thread. If you haven't really changed the subject (and in this case I don't think you have) then creating a new thread invites all this overhead. Nothing you can do about it now, but it's something to think about for next time.
Anybody got a syringe I can use to squeeze the magic smoke back into this?
 

Offline ScribblesOnNapkins

  • Regular Contributor
  • *
  • Posts: 99
Re: PCB-RND
« Reply #48 on: August 16, 2017, 12:37:37 am »
Cerebus you have a point but I don't like the way the threads on kicad stretch off into infinity. It makes them impossible to follow over time. Ether way here is an echo of the new threads only post...


A few days ago we released 1.2.4 which adds some new features. The most notable are...
* Eagle Binary Format - pcb-rnd can now read eagle files in the older binary format. We have a few weeks of testing time in on each release but if you find anything wrong with this please report it to us. We are working on exporting this format as well.
* Protel Autotrax/Easytrax Format - pcb-rnd can now import and export this format.
* Subcircuits - You can now draw a bunch of objects and group them as a subcircuit. This is one of a series of additions in our effort to target microwave/rf users. The next step is making subcircuits have their own distinct terminals and etc in netlist. (I would love it if people would test this but not use it in production until we have more done.)
* xy_exporter - now supports templates (we have a few users interested in using commercial pnp services)

Various bugs were also fixed of course.

To be honest I am more excited about our next 2 or 3 releases than this one not just because of subcircuits but other things (yet to be announced) as well.
 

Offline beduino

  • Contributor
  • Posts: 11
  • Country: 00
Re: PCB-RND
« Reply #49 on: October 30, 2017, 08:58:37 am »
Update:
I've moved this post to better place where pcb-rnd-1.2.6 is discussed, so probaly better place discuss this thing there:
http://www.eevblog.com/forum/geda/pcb-rnd-1-2-6/msg1336004/#msg1336004
« Last Edit: October 30, 2017, 09:14:52 am by beduino »
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf