Re: gEDA-user: gschem: Adding net names to a bus
If you attach the first net to the bus, there's a variable set to the bus object called "ripperdir". If you have a vertical bus and you connect your first net to the upper half, the busripper is drawn below the net. If you draw the first net into the lower half, the busripper is drown above the net. If you have a horizontal bus, the same applies to left and right. See documentation --> file format --> bus, for the variable. And o_net_add_busripper() in file gschem/src/o_net.c for the decision of the ripper direction. Wiw. Thanks! --wpd ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: gschem: Adding net names to a bus
Hi Patrick, On Friday 11 August 2006 04:19, Patrick Doyle wrote: > The other night when I created a bus and attached my nets to it, the > bus rippers were all attached as \. (That is, angled from top to > bottom and left to right). Tonight, for some reason, they seem to be > attaching as /. Did I change something between two nights ago and > tonight? O.k. I've tracked the behaviour. If you attach the first net to the bus, there's a variable set to the bus object called "ripperdir". If you have a vertical bus and you connect your first net to the upper half, the busripper is drawn below the net. If you draw the first net into the lower half, the busripper is drown above the net. If you have a horizontal bus, the same applies to left and right. See documentation --> file format --> bus, for the variable. And o_net_add_busripper() in file gschem/src/o_net.c for the decision of the ripper direction. regards Werner ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: gschem: Adding net names to a bus
1. Draw the bus 2. add one net to the bus 3. add the netname attribute to the net using a wildcard e.g. netname=A? 4. (optional) edit the label properties (alignment, textsize, ...) 5. copy the net (with label and busripper) as many times as you need 6. mark all netnames 7. use the attribute --> autonumber text dialog 8. write "netname=A" to the searchtext and modify the options Thanks... that was what I was looking for. As long as I have your attention, do you mind if I ask another question? The other night when I created a bus and attached my nets to it, the bus rippers were all attached as \. (That is, angled from top to bottom and left to right). Tonight, for some reason, they seem to be attaching as /. Did I change something between two nights ago and tonight? --wpd ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: gschem: Adding net names to a bus
Hi John, Patrick and all, On Tuesday 08 August 2006 15:17, John Luciani wrote: > > As I said, this feels cumbersome, and I thought I would ask if > > there are easier ways to enter in a bunch of similar netnames. > > What I sometimes do is --- > > 1. Create a schematic with a single net. > 2. Edit the netname, font size, name position, etc until the net > appearance is satisfactory. > 3. Copy the net as many times as desired. > 4. Close the schematic and edit net names in EMACS. > A search and replace macro makes this easier. > 5. Use gschem to correct the positioning of misplaced nets and then > copy the net schematic into your main schematic. Here's another way: 1. Draw the bus 2. add one net to the bus 3. add the netname attribute to the net using a wildcard e.g. netname=A? 4. (optional) edit the label properties (alignment, textsize, ...) 5. copy the net (with label and busripper) as many times as you need 6. mark all netnames 7. use the attribute --> autonumber text dialog 8. write "netname=A" to the searchtext and modify the options Note: If you need a top down or a left to right bus this will work fine with the corresponding sort option. If you need a bottom up bus you'll have to place the bus rippers from bottom to top and use the fileorder sort option when renumbering. Regards Werner ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: gschem: Adding net names to a bus
On Tue, 2006-08-08 at 09:17 -0400, John Luciani wrote: > On 8/7/06, Patrick Doyle <[EMAIL PROTECTED]> wrote: > > > So I drew a bus down along side of the symbol and started connecting > > nets to it. So far, so good, but now I want to label the nets, and > > here is where things get a little cumbersome. > > > > Select net, > > aa > > EM_A[...] > > select netname, since it is way to big > > ex > > Change the font size to 6. > > > > As I said, this feels cumbersome, and I thought I would ask if there > > are easier ways to enter in a bunch of similar netnames. > > What I sometimes do is --- > > 1. Create a schematic with a single net. > 2. Edit the netname, font size, name position, etc until the net > appearance is satisfactory. > 3. Copy the net as many times as desired. > 4. Close the schematic and edit net names in EMACS. > A search and replace macro makes this easier. > 5. Use gschem to correct the positioning of misplaced nets and then > copy the net schematic into your main schematic. > > (* jcl *) > What I do is draw one net then set NET=DATA0 for that net then copy and past that net + the bus ripper n times. Finally go down the row of nets and edit each ones attribute. Steve Meier ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: gschem: Adding net names to a bus
> As I said, this feels cumbersome, and I thought I would ask if there > are easier ways to enter in a bunch of similar netnames. What I sometimes do is --- 1. Create a schematic with a single net. 2. Edit the netname, font size, name position, etc until the net appearance is satisfactory. 3. Copy the net as many times as desired. 4. Close the schematic and edit net names in EMACS. A search and replace macro makes this easier. 5. Use gschem to correct the positioning of misplaced nets and then copy the net schematic into your main schematic. (* jcl *) Thanks... I'll keep that in mind. It fits my typical workflow of "I know the tool well enough that I know what tricks I can play with it"... except that I don't know the tool that well yet :-). In the mean time, I'll start dreaming fondly of having enough spare time to add a "net name" menu item to gschem that would put up a dialog box (I never remember the difference between "modal" and "non-modal", but basically the same kind as gets put up when adding a part from a library), prompts the user for a net name, and then allows the user to place it on the schematic, incrementing the numeric part if present. Right now my spare time is devoted to designing a board using EDA tools I've never used before. I'm trying very hard not to allow myself to be too distracted by, "Gee, if only it did this...", in the interest of actually getting the darn thing designed. Thanks again for the tip. --wpd ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: gschem: Adding net names to a bus
On 8/7/06, Patrick Doyle <[EMAIL PROTECTED]> wrote: So I drew a bus down along side of the symbol and started connecting nets to it. So far, so good, but now I want to label the nets, and here is where things get a little cumbersome. Select net, aa EM_A[...] select netname, since it is way to big ex Change the font size to 6. As I said, this feels cumbersome, and I thought I would ask if there are easier ways to enter in a bunch of similar netnames. What I sometimes do is --- 1. Create a schematic with a single net. 2. Edit the netname, font size, name position, etc until the net appearance is satisfactory. 3. Copy the net as many times as desired. 4. Close the schematic and edit net names in EMACS. A search and replace macro makes this easier. 5. Use gschem to correct the positioning of misplaced nets and then copy the net schematic into your main schematic. (* jcl *) -- http://www.luciani.org ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
gEDA-user: gschem: Adding net names to a bus
I've read the gschem documentation (only) enough to read the part that says "buses are still very experimental". Nevertheless, I thought I would give it a try. I have a symbol that I've imported has a bunch o' pins labeled: EM_A[0] EM_A[1] EM_A[2] ... So I drew a bus down along side of the symbol and started connecting nets to it. So far, so good, but now I want to label the nets, and here is where things get a little cumbersome. Select net, aa EM_A[...] select netname, since it is way to big ex Change the font size to 6. As I said, this feels cumbersome, and I thought I would ask if there are easier ways to enter in a bunch of similar netnames. I expect I can change the default text size (pokes around a little and finds "ot"). But I still wonder if there is an easier way. Actually, the same question applies to having drawn the nets connections to the bus itself. Is there some way I could draw the line once and repeat/redo it down the line? Note that, since this is an imported symbol, I'm not sure that the pins are on the default grid or not (but I can fix that in the future). --wpd ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
