Need a pin renumbering tool

[eric_engineer]

In footprint editor I need a fast renumbering tool so I don't have to manually edit 100 pins on this part right now.  Something like start from this pin and renumber counter clockwise. Or let me start at one pin and just click through and renumber them in sequence automatically (without telling me the pin number already exists).

Thank you

[eric_engineer]

Woah.  So I just manually renumbered these pads in the footprint and instead of my schematic mapping -> footprint pins staying the same... It changed them behind my back, I guess to keep the same pin to pad regardless of the fact that I just changed the pin number!  So now the part doesn't match again and I have to manually re-assign.  I claim this is bad behavior.

[chuck_toddN7PTC]

I agree, this would be useful.

BR - Chuck

[eric_engineer]

Going to add one more thing to this. So I manually disconnected and then properly reconnected all the pins on this device at the component level. Saved it.  Then went to schematic and layout and updated library.  Most of it worked but the tool assigned the GND net to one of my disconnected signal pins. I verified I had set it to the right signal name when connecting and it was the right pad name in the schematic.  When I restarted fusion and came back in it was fixed. There's a consistency bug there for sure.

[jorge_garcia]

Hi @eric_engineer ,

I hope you're doing well. So to the first point, If a part is fully connected and you change the name of some pins/pads do you want the connections to automatically change? Perhaps in this case, but in other scenarios it can cause a working component to be incorrect. The devs took the most conservative approach which is to preserve the connections until they are explicitly remade regardless of any naming changes. It's a safe behavior, even if in this scenario it didn't match your expectation.

I fully agree with a renumbering tool in the footprint editor. We are working on a renumbering tool for the electronic design, so maybe some of that work can be used to implement this. One thing you can do to make these types of tasks easier is to check out pin/smd/pad array commands or the make-device-symbol-package-bsdl.ulp that comes with Fusion.

The last comment about inconsistency is concerning, if it happens again please let me know.

Best Regards,

[eric_engineer]

The whole manual connecting of pad to schematic pin approach is one of my least favorite things about Fusion. It is very error prone and concerns me every time I have to do it. Putting that aside, I see what you are saying about developers trying to be conservative with a "the user didn't explicitly change this approach". In this case I almost released a board with the wrong footprint, it was only because something felt off when I went back in to route that I noticed it.  I'd argue that previously I took a user action to define schematic pin A0 = Pin 1 in the component tool, and you should honor that even if I decide to change the numbering in the footprint. I made my assignment name -> number, not name to underlying representation of a specific pad in software 😉  If we had a renumbering tool I'd expect Fusion to also honor my previous schematic -> pad assignments.

[jorge_garcia]

Hi @eric_engineer ,

"The whole manual connecting of pad to schematic pin approach is one of my least favorite things about Fusion. It is very error prone and concerns me every time I have to do it."

I'm curious what alternative have you experienced when making your own components? The make ULP I mentioned above can take a BSDL file and generate a full component from that. Happy to hear your ideas.

Let me know if there's anything else I can do for you.

Best Regards,

[chuck_toddN7PTC]

This is the workflow I used for making library components prior to Eagle/Fusion.

Pins in the schematic symbol automatically associate with the pads in the footprint based on the pin/pad number.

Importing Library

https://youtu.be/a8UG1_U1KtU?si=JWpmRp7keQA57QTn

Manual library creation with IPC footprint wizard

https://youtu.be/bOi45nshqP8?si=ZSB60sA8Ig1C7JvF

BR -Chuck

[jorge_garcia]

Hi @chuck_toddN7PTC ,

Thanks for sharing the videos. Lots of respect for Robert Feranec, he makes great videos, fully agree with him when he says "If you import a component always verify it". So true...

Looking at the videos the key difference in library structure between Altium and Fusion becomes clear. Altium avoids the connect dialog by including the pad number as part of the symbol along with pin name. The downside to this approach is that it limits symbol reuse, since in multi-gated components you can't just use the same symbol for every gate without modification. If you are trying to re-use a symbol with a different component you'll have to modify the pad number in the symbol. Fusion maintains a separation between the schematic and footprint realms by relying on the Connect dialog in the component definition to map. Obviously both approaches work, it's just a matter of what you are used to and prefer. 

If most of the time you are importing components from third parties like in the Feranec video the difference really isn't that critical. In Fusion you can use the SnapEDA and Ultra-librarian plugins to download parts from third-parties. I do really like the distributor integration that Altium has, we have that on the todo list. Currently, that's why we rely on third party plugins to achieve part of that functionality but a fully integrated solution would be ideal. You don't have to use a copy and paste workflow like Robert showed, you can use the part straight from the downloaded library or import them into your own libraries through the import command.

Fusion contains an IPC complaint footprint wizard similar to the one in Altium, it will generate both the footprint and 3D model for you.

If there is a specific part that's giving you trouble feel free to reach out.

Thanks again for sharing the videos.

Best Regards,

[eric_engineer]

Manual way, least preferred

I agree with Chuck, other tools usually use a pin number defined in the schematic pins defined in the footprint. I get that Fusion does it different, but it's really easy to make a mistake in that totally separate popup window where you can't even see the schematics symbol or your footprint and you have to manually select each pin to pad.  Hope you don't click the wrong one or accidentally select two or something 😉  And yes we always verify in design review but that's not the answer.

Auto table based, better

The manual approach is a last resort though. In other tools we just open the datasheet, and copy the pin table into excel then set all pin attributes (passive, output, I'm a clock etc, size, side of part etc). Drop that table into the tool which auto-generates an initial symbol and then I drag the pins around to be where I want. But the key thing here is I didn't spend ten minutes typing in pin names and assigning numbers. I didn't make a mistake fat fingering a pin number because it's right from the datasheet. I have it in excel in case I messed up and need to change something after import. And then like fusion I can use the IPC footprint generation tool and I have a full part.

I could see a fusion feature where you let me copy in a pin name -> pad mapping from a datasheet like that. It would still work with your flow.  Maybe I could define the footprint first, copy and paste my table and get a symbol auto generated that I could then edit. 

Oh and BSDL, we don't even use that as an output from our FPGA tools anymore. And you can't get it for most parts anyway so table input is much better.

SNAP & Ultra

I also agree with you that nowadays I'm going to start with Snap or Ultra first. Here though your integration is not tight enough. I think Snap has a  good flow, but it always imports it into a SnapEDA library, not my organized library(s), and not with my attributes. So there's always the extra step of importing it from snap, and then manually going and setting the attributes to what we need, now open the right library, import, find the part in snap.  It's slow.  

Real Library flow

And I don't want to go too off topic but library management in Fusion is sorely lacking compared to other tools. We do real-part driven design, so in other tools I'll find a part on digi, arrow, mouser, etc. I drop the part number into my tool and it two clicks I've added a new resistor backed by a real part number. And then later searching, it's so easy in our other tools to quickly find a 2uF 201 cap in our database and drop it into the design. The old approach of manually dropping a generic cap and assigning it a value is for the birds 🙂 We fake it in fusion with libraries and naming  conventions but I don't like it.

My continuing complaint about using Fusion Electronics professionally is it puts a lot of burden on the  user and tasks that are quick and simple in other tools require me to take on too much. To the point I hate to have to add a new part in Fusion. Even to just duplicate a real resistor in our Fusion library you have to duplicated it and change four sections to get it right name, description, parameters. This takes time and it's easy to make mistakes. It's not

I will say that so far the Fusion team has been very responsive to complaints / feature request and I've seen some things I asked for actually roll out. So I do appreciate that.

[chuck_toddN7PTC]

I agree with @eric_engineer 's comment.

Quoted below:

"My continuing complaint about using Fusion Electronics professionally is it puts a lot of burden on the  user and tasks that are quick and simple in other tools require me to take on too much. To the point I hate to have to add a new part in Fusion. Even to just duplicate a real resistor in our Fusion library you have to duplicated it and change four sections to get it right name, description, parameters. This takes time and it's easy to make mistakes. It's not"‼️👏

Too much time is spent in the library and that cuts into design time. Component generation needs to be streamlined.

I know this is a common hardware engineer response, but "it's just software". 😉

------------------------------------------------------------------------------------------------------------------------------------------ 

I have attached the most recent high density processor I had to use. This is an example of what we need assistance with making connections between the symbol and footprint.

Schematic symbols A - R, Footprint with 425 pins. Manually making these connections was extremely tedious.😰

      

BR -Chuck

[jorge_garcia]

Hi @eric_engineer and @chuck_toddN7PTC ,

Thanks for the continued feedback. I'm going to try to answer things in order, if I don't mention something it's because it's a legitimate need.

First to @eric_engineer 

There is a table based sort of approach available, unfortunately it's not super discoverable. It's super useful for making symbols and it relies on ripping the info from the datasheet. It's called Smart Paste, we have shown it in a webinar and in an old video which I have linked here. It doesn't quite go all the way to making the connections of the component but it speeds up symbol creation considerably. Check it out, I think this is close to what you are suggesting and probably wouldn't take much to have it go all the way.

https://www.youtube.com/watch?v=0wNLXXT_jsA

Our biggest lack is in the Real Library flow department. With a stronger BOM implementation we could get a lot of that info into the libraries or update it in the schematic when things like pricing info change. Agree here.

Also agree with you that the SnapEDA and Ultralibrarian plugins need to be better integrated.

@chuck_toddN7PTC 

I'm so sorry about that. I know @eric_engineer mentioned that he doesn't use BSDL files anymore, but high pin count devices often provide them. The BSDL file can actually be used to make everything symbol, footprint and the component connections. When used you'll get one big symbol. We have another tool that can be used to break the big symbol up into smaller symbols. These are tools from the EAGLE days, they work but are not the most polished.

If you constantly have to make parts like this I encourage you to give them a try. I'm happy to walk you through the process, unfortunately we don't have any videos of that workflow although documentation is available.

Best Regards,

[chuck_toddN7PTC]

@jorge_garcia 

Can you provide more information about the other EAGLE tool that you mentioned for breaking symbols into to smaller sections? Documentation?

I would like to try the BSDL method for making larger parts to see how that may improve the workflow.

BR -Chuck

[jorge_garcia]

Hello @chuck_toddN7PTC ,

I've attached the documentation for the 2 ULPs, the make-symbol-device-package-bsdl. ULP is the main mover, it can process the BSDL or other text file to create complex components. The connect-device-split-symbol.ulp is the one to use to break a large symbol into smaller pieces.

Let me know if you have any questions.

Best Regards,