As to the old question of how Protel treats pads with the same name/number: we don't know for sure, and cannot find out. And anything we assume is likely to become incorrect across versions. So it's best to use unique pin names/numbers.
Perhaps. First of all, it is quite clear how a CAD system should handle duplicate pin numbers. It should assign the same net to both pins. There is no other legitimate meaning for duplicate pad numbers: they are electrically identical, perhaps because they are necessarily connected by the inserted part, or because they are part of a complex pad structure.
A common example would be a BNC connector with four ground pins. When the part is inserted, all four pins are connected together whether they are or are not connected together. The common schematic symbol for a BNC connector only has two pins. There are two ways to handle this:
(1) create a new symbol for the connector which has four ground pins, each with a unique name. This is the Bagotronix solution.
(2) use the classic symbol and place four ground pads in the BNC footprint.
I find the second option much less cumbersome. For one thing, I'm going to continue to receive schematics and netlists from engineers who are going to have two-pin symbols, i.e., only two pins in the netlist, and I'm not the only one. Only if you have control of both the schematic and the PCB is the first option reasonable.
Now, I just checked DXP behavior. I did not check all aspects of the behavior, for sure, but I found that if I made a footprint with a double pad, placed it on the PCB, used a part with only a single pad on the schematic, that pad being wired, DXP correctly assigned the same net to both pads.
I then reran the update from schematic. No change, which is correct. So far so good.
HOWEVER, Altium still didn't get it right. This is a bit irritating, since this matter has received a lot of virtual ink over the years.
I removed the net assignment from one of the pads and reupdated. Schematic incorrectly reported that there were no changes.
Then I deleted one of the wires on the schematic. This wire was connecting two of these double-padded parts. Updating the PCB correctly removed -- or attempted to remove -- the net involved. However, it only removed net assignments from one of the pin sets, the other maintained the net assignment (for both pads). This, however, is an unrelated problem: non-double-padded parts show the same behavior (a single node net is left, which is not correct).
This is DXP SP2, BTW, fresh off of a new CD, I have not checked into further service packs, and I don't know if this has been discussed on the DXP list, since I've been off of it for a long time. (I'll go back....)
Exporting a netlist from the board produced double mentions of the pads, as might be expected. (I'm not sure if this is the best behavior, but at least it is quite reasonable; further use of that netlist would have to handle or eliminate duplicates.)
While the behavior is a little buggy, it still functions correctly unless I toss it a curve ball by manually editing pin nets. Further, if the double pads are wired together in the footprint, DRC will catch any anomalies.
Now, what happens with net list load? Unfortunately, I had trouble testing this as I could not readily find a means to import a net list into DXP. If all else fails, read the manual, and check out the Protel web Knowledge Base....
Ugh. Complicated. Powerful, yes, simple, no. That seems to be a DXP refrain. Unfortunately, OrCAD Layout had the same problem, part of the Protel advantage was intuitive interface, simplicity of use. All this could be corrected rather easily by adding in alternate paths of use that will be quickly found by a prior user....
I do think the DXP way is, in the long run, better. But, hey, how about considering your loyal users when you change the program? It would not take much to build in legacy methods, even if they only pop up a dialog saying "this process has been replaced with ...." And then there could be a control somewhere that removes or adds the legacy buttons or commands. The biggest complaint I have seen about DXP (in the Forum) has been its complexity....
In the process to import a netlist using "Show Differences," there is a necessity to right-click in a dialog box to pull up a menu. Actually, there are two of these, the first one just to find "Show Differences." Remember the famous hidden "Update Free Primitives from Component Pads"? It appears that the lesson was not learned. When there are advanced menus, there ought to be an indication that they exist!
Anyway, double pads work well enough; in fact, netlist load now functions the same as update from schematic. And as far as future versions, I can hope that the remaining problems will be fixed. No way should pads with the same logical name -- except for free pads and no-name pads -- have different nets. Ever.
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
