[kicad-users] Re: Pcbnew Problems
Dick, I took your advice on the changes to the way the mouse works. I renamed the schematic and generated a new net list and then read it into PCBNEW. Everything worked fine. I had become accustomed to working with the mouse the way it used to work. I think the difference in the OnClick and OnRelease is what got me. Thanks for the Advice --- In kicad-users@yahoogroups.com, Dick H. [EMAIL PROTECTED] wrote: --- In kicad-users@yahoogroups.com, daystar1013 daystar@ wrote: I use kicad daily for reverse engineeering and occasionally PCBNEW for test fixtures. I have been using the 2007-11-29-RC2 release for Windows, I have not layed out a PCB until today. I started a PCB layout, a small circuit (5X3) with six - 16 pin SO14E footprints and two TQFP-44's, 1206 resistors and capacitors, and some LEDs. I read the netlist into pcbnew and as usual the parts were all stacked up on top of each other, no problem. I place the parts manually, I do the entire process manually, PCBNEW is an excellent tool for manually routing a PCB. The problem I started seeing was that I would move a part, and place it. I would go to move the next part, and I would grab the same part off of the stack that I just placed. About half the time a part I placed would stay where I placed it. I finally gave up and went back to the July release. I completed the board in a couple of hours. One of the changes we made in this release involves mouse clicking. (And for a good reason I'll add right up front. There is no going back.) Many of the program's actions happen now on the mouse release, whereas they used to happen on a mouse press. So you might look at what makes up your environment, including your mouse driver, your mouse, and your version of Windows. Also consider how you are using the mouse. Try slowing down and verifying that when you drop the footprint in place, it stays there. Others do not seem to be having this problem.
Re: [kicad-users] Re: PCBNew Problems
Dick H. wrote: It was choking on a bad layer number in the REFERENCE text of your PIC footprint. I'll now go see where the layer number is coming from, but my change will get you by. I can't see anything in the code. You should probably manually edit your *.brd file with a text editor and set your layer numbers for all your T0 and T1 texts to a reasonable number. Thanks for the help and information. I'll look at the file, but I don't know what T0 and T1 texts are. I'm not only new to kicad but to board layout and schematic editing as well. This is the first circuit I've ever designed and the first board layout I've ever done so I may not know quite a bit of stuff! Programming I have done though and I'd like to dig into the kicad code when I get some time. The value of 21 is predominant as you can see elsewhere in the file. And from include/pcbstruct.h, we have this to support that idea: #define SILKSCREEN_N_CMP 21 Dick Hollenbeck SoftPLC Corporation http://softplc.com
[kicad-users] Re: Pcbnew Problems
--- In kicad-users@yahoogroups.com, daystar1013 [EMAIL PROTECTED] wrote: I use kicad daily for reverse engineeering and occasionally PCBNEW for test fixtures. I have been using the 2007-11-29-RC2 release for Windows, I have not layed out a PCB until today. I started a PCB layout, a small circuit (5X3) with six - 16 pin SO14E footprints and two TQFP-44's, 1206 resistors and capacitors, and some LEDs. I read the netlist into pcbnew and as usual the parts were all stacked up on top of each other, no problem. I place the parts manually, I do the entire process manually, PCBNEW is an excellent tool for manually routing a PCB. The problem I started seeing was that I would move a part, and place it. I would go to move the next part, and I would grab the same part off of the stack that I just placed. About half the time a part I placed would stay where I placed it. I finally gave up and went back to the July release. I completed the board in a couple of hours. One of the changes we made in this release involves mouse clicking. (And for a good reason I'll add right up front. There is no going back.) Many of the program's actions happen now on the mouse release, whereas they used to happen on a mouse press. So you might look at what makes up your environment, including your mouse driver, your mouse, and your version of Windows. Also consider how you are using the mouse. Try slowing down and verifying that when you drop the footprint in place, it stays there. Others do not seem to be having this problem.
Re: [kicad-users] Re: PCBNew Problems
Moses McKnight a écrit : Dick H. wrote: 2) Can email me your board files with exact instructions on the menu choices you use to reproduce the problem? I'm willing to spend 15 minutes on the problem, so don't blow that time with less than specific instructions please. Do I need to send the any module libraries or are the modules embedded in the board file? As I mentioned I did get a previous version to plot the files, but I'll send you the file anyhow in case you want to look at it for debugging. If not already done, send the .brd file (no other file is needed) to Dick or to me -- Jean-Pierre CHARRAS Maître de conférences Directeur d'études 2ieme année. Génie Electrique et Informatique Industrielle 2 Institut Universitaire de Technologie 1 de Grenoble BP 67, 38402 St Martin d'Heres Cedex Recherche : GIPSA-LIS - INPG 46, Avenue Félix Viallet 38031 Grenoble cedex
Re: [kicad-users] Re: PCBNew Problems
Moses McKnight wrote: I've attached the file. Hope it helps for debugging. Thanks, Moses Re: seg fault when plotting. OK, I checked in a fix for this at SVN. It was choking on a bad layer number in the REFERENCE text of your PIC footprint. I'll now go see where the layer number is coming from, but my change will get you by. Dick
Re: [kicad-users] Re: PCBNew Problems
On 8 Dec 2007 at 12:02, Moses McKnight wrote: BTW, where is a good place to get prototypes made inexpensively with solder mask? I'm looking at pcbfabexpress.com right now but am interested in other options. Thanks, Moses I get mine done at http://4pcb.com They have a $33 special. That is $33 each (min order of 3) for any size up to 60 sq. in. double sided including solder mask and silkscreen on both sides. You can put mutliple board designs, but it must be a single part number and for that price, they will not cut them apart. I always put as many of my prototype designs as will fit in 60 sq-in and then cut them apart with an 18 paper cutter. Dave - WB6DHW http://wb6dhw.com
Re: [kicad-users] Re: PCBNew Problems
[EMAIL PROTECTED] wrote: On 8 Dec 2007 at 12:02, Moses McKnight wrote: BTW, where is a good place to get prototypes made inexpensively with solder mask? I'm looking at pcbfabexpress.com right now but am interested in other options. Thanks, Moses I get mine done at http://4pcb.com They have a $33 special. That is $33 each (min order of 3) for any size up to 60 sq. in. double sided including solder mask and silkscreen on both sides. You can put mutliple board designs, but it must be a single part number and for that price, they will not cut them apart. I always put as many of my prototype designs as will fit in 60 sq-in and then cut them apart with an 18 paper cutter. Dave - WB6DHW http://wb6dhw.com Hmmm, wonder if I can put three or four of the same board on a panel? How would I do that with Kicad anyhow? The min order of 3 panels would get me right now as I need on 2 or 3 boards and cost is an issue. I will probably change later boards but the first ones will be for development and will work for what I need right now. Thanks, Moses
Re: [kicad-users] Re: PCBNew Problems
Moses McKnight wrote: [EMAIL PROTECTED] wrote: They have a $33 special. That is $33 each (min order of 3) for any size up to 60 sq. in. double sided Hmmm, wonder if I can put three or four of the same board on a panel? How would I do that with Kicad anyhow? The min order of 3 panels would get me right now as I need on 2 or 3 boards and cost is an issue. I will probably change later boards but the first ones will be for development and will work for what I need right now. If that special doesn't match, custompcb.com does 8x10 mini panels with a min order of two for about $70 shipped no frills not too too many holes, no silk, no mask, and you can add another mini panel easily to get more...probably = $30. John G
Re: [kicad-users] Re: PCBNew Problems
On 8 Dec 2007 at 14:21, Moses McKnight wrote: [EMAIL PROTECTED] wrote: On 8 Dec 2007 at 12:02, Moses McKnight wrote: BTW, where is a good place to get prototypes made inexpensively with solder mask? I'm looking at pcbfabexpress.com right now but am interested in other options. Thanks, Moses I get mine done at http://4pcb.com They have a $33 special. That is $33 each (min order of 3) for any size up to 60 sq. in. double sided including solder mask and silkscreen on both sides. You can put mutliple board designs, but it must be a single part number and for that price, they will not cut them apart. I always put as many of my prototype designs as will fit in 60 sq-in and then cut them apart with an 18 paper cutter. Dave - WB6DHW http://wb6dhw.com Hmmm, wonder if I can put three or four of the same board on a panel? How would I do that with Kicad anyhow? The min order of 3 panels would get me right now as I need on 2 or 3 boards and cost is an issue. I will probably change later boards but the first ones will be for development and will work for what I need right now. Thanks, Moses Yes, I do that. Make up a new board that will be 60 sq-in. From the File Menu, select Append Board and navigate to the board you want to place. You can then use the block copy to make more than one copy on the board. You can also import other board designs with the Append Board command. I use a combination to fill up the 60 sq-in. By the way, 4pcb.com also has a free service that checks your Gerbers for manufacturing errors before you even order. Dave - WB6DHW http://wb6dhw.com
[kicad-users] Re: PCBNew Problems
The other problem is that when I run a DRC check it says a number of pads are unconnected which are not unconnected. I did not have this problem when I ran a DRC a little while back, and the only thing I've done since then is increase the size of my vias and move some runs around. It would also plot without problems before. So how do I tell PCBNew that the pads are connected which have traces going to them? The Nov-2007 release has the Selection Clarification menu which you get when you click over your pad/track combo, right above the pad. In this menu you can see all the track segments which are under the mouse. (Using the hollow track display mode also helps see all the segments at or near the pad.) But back to the menu, your choices will show the net number and/or name next to any track segment. If you see a net number of 0 this means that segment is not connected as far as pcbnew is concerned. (Your disagreement with its understanding does not change its interpretation.) The segment has been lost to the scrap heap and should be deleted and re-entered. You have to delete that segment and re-enter it. The problem is that pcbnew uses segment end point testing to detect continuity, rather than visual overlapping. During track entry, visual overlapping is sufficient to cause the injection of small segments behind the scenes to actually achieve precise end point equality. End point equality is when pointA.x == pointB.xpointA.y == pointB.y exactly. So the end point of one segment must *exactly* match the endpoint of the next segment for there to be continuity. During track entry, things are happening behind the scenes to add small short segments to tie all the segments together *exactly*. However, if just one of those segments is moved later, or a pad as a result of a suttle footprint move, then there is no similar support for *repairing* the end point equality. This small segment injecting is only during track entry. A similar discussion relates to the last segment on a track, the one that connects to the pad. Here the exact (x,y) match also must be true for one of the last segment's 2 end points as it compares to the centerpoint of the pad. I am only the messenger, please don't shoot me. There has been some discussion about relaxing the end point equality checking and going with a do they overlap type test. I am in favor of that now that computers are faster. The computer should work for us, not the other way around. And to me, if it looks like two track segments are overlapping, then I'll bet that the same thing in copper would conduct electrons :). The original design was done to speed up the ratsnest algorithms, where the end point equality test was the fastest among any other alternative test. With upcoming zone re-design, this end point equality test is back on the table for discussion. Dick Hollenbeck SoftPLC Corporation http://softplc.com
Re: [kicad-users] Re: PCBNew Problems
During track entry, things are happening behind the scenes to add small short segments to tie all the segments together *exactly*. However, if just one of those segments is moved later, or a pad as a result of a suttle footprint move, then there is no similar support for *repairing* the end point equality. This small segment injecting is only during track entry. I use an independent Gerber viewer to double-check Gerbers, which sometimes reports that there is a zero length track at x,y. Could the short segments you refer to be the cause of that? Being zero length and almost invariably hidden underneath something else they are a pig to find back in PCBNew, even though the Gerber viewer reports their precise location. Regards, Robert. -- No virus found in this outgoing message. Checked by AVG Free Edition. Version: 7.5.503 / Virus Database: 269.16.17/1176 - Release Date: 12/6/2007 23:15
[kicad-users] Re: PCBNew Problems
So how do I tell PCBNew that the pads are connected which have traces going to them In the case where the last segment of a track is actually connected to a pad using exact end point matching criteria, and the only problem is that the net code for the track is 0, then you have an additional remedy. Look at the menu option Track Operations. In there is a checkbox called Connect to Pads. This will update the net code on that last segment from 0 (meaning unconnected) to the net code of the pad, but only if it is truly connected according to pcbnew's (too) strict criterion: the endpoint of the last track segment must exactly match the center point of the pad. You can use any of the track operations to help clean up your board, including the Connect to Pads option exclusive of the others, which is what you should try first. Hope this helps. Dick Hollenbeck SoftPLC Corporation http://softplc.com
