PADS Logic has a Signal Pins function, where you can connect pins not shown on the decal by net name. Select the part in Logic, open the properties dialog, you will see a signal pins button. This is not the most elegant solution, and actually can easily lead to errors, but it's an option. I would much prefer Mentor offer a way to logically connect the signal pin to another pin in the library editor, not relying on manual connections when creating or modifying a schematic. If anyone else has a workaround, I'd like to hear it.
That said, pins that might need to be probed in testing/troubleshooting, like relay pins, really should be shown on a schematic. All connector pins MUST be shown on a schematic, the exeption being (this might be your case) where there are two soldered connections on the board for each off board pin. I'm glad to hear there are still people who are concerned with the way their schematic looks. Too many engineers don't realizxe that the people trying to read those schematics for years after they are done with them aren't so familiar with teh circuit and need an easily readable schematic. You can mainain that with multiple pin connections. If you are showing the relay as an analog symbol, just make sure you show the wiper pins internally connected.
Thanks for the info, Pete.
I talked to a guy from the sales office yesterday who gave me the same fix for my issue.
I tried it this AM with the relay and it works OK.
I had to go into Layout and in ECO mode, add the connection for the pin, but it seems to work.
PCAD, for what it's worth, allowed you to "jumper" pins in the Pins dialog box during part creation/editing.
The pins were equal in the netlist.
Can I ask you another related question?
Are there any reasons why I can't create a part type that is, in real life, a connector?
For the 1/4" male/female quick connect tabs on my board, I have created new part types for these two connectors, instead of creating them as connectors.
If I create them as connectors, I can't make the second pin a signal pin.
Also, I do not have multi-sheet schematics involved, so I do not need connectivity across sheets.
Lastly, thanks for the kudos re:drawing good schematics.
My philospohy is I try to draw my schematics to AID the person who might have to read them, not to confuse him (or, her).
Otherwise I am not doing my job.
Well, Pete, I tried it.
I have to do some more experimentation in the Parts Editor to get the nets to connect properly, but I was able to get the relay to load into Layout without a net connected to it.
Then I was able to make a connection between that pin and the correct net.
I have to do some fooling around with pin swapping in the Parts Editor to get my other parts working right.
It is just a workaround, but I will keep fiddling with it.
I also thought about placing a trace between the two pins involved in the PCB decal.
I think I will fool around with this also, to see which solution seems to work best with my design.
Thanks for the info.
I do sometimes create connectors as part types, it depends on function, schematic connections, etc. It can be useful for 10 pin connectors, not so much for 100 pins.
You can add your duplicate connections to teh LAyout, but then when you make schematic changes and use the PADS Layout link to update the board, your Layout mods are lost.
Adding the connection in the decal is problematic, because it creates a built in DRC error. If it's a SMT connector, you could use associated copper to make 2 cionnected pads for 1 pin.
It would be nice if PADS could put a coupled pins feature in the next update, but don't expect a lot of improvements to PADS Logic. Mentor has been trying to migrate PADS users to DxDesigner for years.
With PCAD2006, connectors are just parts like any other, so I am used to this sort of thing.
I think I will start exploring this.
I have gotten the feeling that Mentor didn't want us to use PADS Logic.
I started out trying to use DxDesigner, but right away I found out that I needed the library management application for DxDesigner, too.
We talked to Mentor, and they told us that we had to buy a library management program for DxDesigner.
They told us that the PADS ES suite didn't come with this, that it was an add-on.
So, we decided to use PADS Logic, as our circuits are pretty simple ones.
Thanks again for the info, Pete.
1 of 1 people found this helpful
You need to get past some assumptions you're making, and some pre-conceived notions from a former tool.
PADS' connector type of symbol is simply a built-in shortcut. I never use it myself. It is not required, and any connector can be made as a regular part.
Professional schematics show every electrical connection, even if it's internally connected within a part. The relay is no different than a 1000 pin BGA, in that every ground connection needs to be shown as connected. Making it readable is your task. My standard is one could derive a 100% correct netlist just from tracing out a schematic printout.
Hiding pins and connections with an signal net, or PCAD's jumper option is not a good idea (I've used PCAD since 1987). These are throwback concepts were designed to make CAD drawn schematics look like hand-drawn, where connections like power and ground pins were left off for clarity and ease of drawing. That's so last century.
I can trace 80% of the netlist packaging errors, especially with PCAD, to the use of the hidden signal pin and jumper options. Most of the time, they came from reusing an old schematic, and the engineer forgets to change all of the hidden pins. Back annotating in PCAD failed because the jumper pin option was not supported by their schematic. And in the bigger picture, translation between different CAD tools might fail when these options are used, or almost worse, works with undetected errors.
You know, David, you brought up some good points, and you made me think about the true intent of the schematic.
I appreciate that.
It is too easy to forget, and get off on tangents.
I think you are right about hidden pins, and the fact that they are hidden can easily lead to errors.
I will have to go back and revisit my parts.
I have always thought that, for example, power supply pins should be shown in a schematic, and not hidden.
Those "floating" bypass caps look so silly just hanging out by themselves!
I also appreciate your thoughts on connectors in PADS.
And yes, I am very "used to" PCAD, because that was the tool we chose at my old job way back, when it was DOS Tango Sch & PCB-about 20 years now.
I was able to get PCAD to do everything I needed to do, and now, I feel very inadequate while using PADS.
Since I've only been using PADS for a couple of weeks, I just need some time using PADS to gain the confidence I have in PCAD.
Thanks to both of you for your thoughts.
Thanks for taking my comments in the spirit they were meant. I have a tendency to come off a little snarky, and I usually don't mean it.
Not snarky at all, very pertinent.
Many years ago, when we started using PADS to replace hand drawn, I had a very hard time convincing the engineers and designers to show all of the supply and drain pins on the schematic. Some didn't even want to show bypass caps, because, you just KNOW they are there.
I do use the PADs signal pin feature, but only for situations where there are pins that do not have an electrical function, but want to be referenced to a GND. Yes, I've missed a gnd on a thermal pad on rare occasion, but not one that stopped a circuit from functioning. It would be nearly risk free if Mentor would offer a way to associate pins, rather than using signal pins. There are some parts that use multiple physical pins for each connection, like in this situation. Mechanical requirements create 2 pins that are externally connected to create the logical connection. But the general rule is, if it has any electrical function, it goes on the schematic.
As for the PADS connector part type - it really shouldn't be part of this discussion since signal pins aren't available on connector parts. They are helpful. Rather than building a single 100 pin connector and spreading off page symbols all over the schematic, you can place an individual pin right at the source, and not have to move around the schematic to find which pin is the desired signal.
I don't mean to steal the thread, but that's the first valuable description of a connector component that I've seen in my many years of using PADS. Thanks, Pete! I had written them off as useless a long time ago. Now I'll have to revisit them. Maybe you should write manuals for Mentor!
I really appreciate all of the comments.
After reading what you guys have all written, I think I am going to set up most of my connectors as regular part types, because I don't have the issue of large pin count connectors in my circuits.
Been a while, but I wanted to thank all of you, because I really wouldn't have any way to find out this stuff other than trying it out myself, which takes time.
The advice you all have given me saved me that time.
So, "Thank you!".