Showing the footprint name on the schematic

[thmjpr]

Whenever you have a component with multiple footprints available, its possible to have the wrong footprint selected.
Is there any way to show the name of the footprint on the schematic somehow? Of course without manually entering it, it would be linked to the selected footprint.

From the help page on Parameters it sounds like this is not possible: https://www.altium.com/documentation/18.0/display/ADES/Sch_Obj-Parameter((Parameter))_AD

Several system parameters cannot be made visible (and be selected) on a schematic sheet, and are therefore not available to the Parameters mode of the Properties panel. For component objects, these are Description, Design Item ID, Footprint, model references and so on. Other system parameters that are not directly accessible in a schematic include Document (Sheet) and Project parameters.

Quick search didn't find anyone else asking the same question so I'm thinking most people are dealing with unique component libraries (ie one 0603 10k part).

=footprint doesn't work.

[T3sl4co1l]

Just review them in the footprint manager (T, G) or copy the parameters with the parameter manager (T, R).

Tim

[bob91343]

That's why we have parts lists in addition to schematic diagrams.

[thmjpr]

Just review them in the footprint manager (T, G) or copy the parameters with the parameter manager (T, R).

Tim

thanks, yeah thats probably the only way to see and review them.

That's why we have parts lists in addition to schematic diagrams.

I understand parts lists are a thing, but they have no location context, unless you want to cross-reference each part which takes time.
I think it could be a useful feature for quick review/design review. Something like: Toggle footprint display -> then look through your schematic -> oh 0402 part next to a regulator, that seems too small, etc.
Yes you could do this on the PCB, but then you'd would want to enable "value" params as well.

[bob91343]

Pardon my senior moment, but I once again forgot what the number means.  I know it's the dimension but forget how.

[T3sl4co1l]

Y'mean size codes?  Usually 0402 ~= 0.04" long x 0.02" wide, or 1608 = 1.6 x 0.8 mm, but watch out for codes that are common to both measurement systems.

Tim

[bob91343]

Aha!  That explains why I couldn't remember the code.  It's because there isn't one, but more than one.

Whose idea was this?  In most electrical engineering work, inches are not the preferred dimension unit.  But it's a hybrid world.  I just purchased a Chinese caliper that has a button to toggle between metric and English systems.  Incidentally, that device is some kind of bargain, very precise and only around $3.

[ddavidebor]

The issue here is another. To avoid mistaking the component, you should identify your components by the full manufacturer part number.
Example: AD8605 vs AD8605ARTZ

That's also because components are not equal. Apart from potentially different pinouts, thermal resistance of each package, and different performance of the component (many components have "A" and "B" variants where "A" is more precise for example), short codes do not identify the component well when it's a fairly generic one.

For example LM324 is a popular opamp. Everyone makes an opamp called LM324, but for example many chinese companies do compatible variants based on a CMOS process that are somewhat compatible, but with very different performance than LM324 from ST or TI.

Similarly, packages are not equal. MSSOP for example are provided in various width by different manufacturers.

[free_electron]

1 part = 1 symbol + 1 footprint + same footprint [manufacturer(s)+ordercode(s) ]

i have in my library the following parts:
LM324-DIL
LM324-TSSOP
LM324-SO
LM324-SON3x2

in my schematic library there is
IC-GENERIC-QUAD_OPAMP_LM324STYLE  (used for all parts , except the SON body since that has an extra pin)
IC-GENERIC-QUAD_OPAMP_LM324STYLE-15PIN (SON flavor with extra pin

In my pcb library there is
DIL14
SO127P490-14N   (SO Package 1.27mm pin pitch , 4.9mm toe-to-toe, 14 pins)
SO65P310-14N     (SO Package 0.65mm pin pitch , 3.1mm toe-to-toe, 14 pins)
SON50P300x200-14-T150x200 (SON package 0.5mm pitch, body 3.0x2.0 mm 14 pin , thermal pad 1.5 by 2mm)

Whatever i drop on the schematic will have correct information attached. the footprint, symbols and manufacturer/manufacturer order codes will be correct.

Set it up right in your library, once , and you never need to worry about it.

Same for resistors.
Simply make those with a unique footprint attached. I encode the footprint hard in the symbol.

Make a spreadsheet with the data
1 column value, one column wattage, one column tolerance, one footprint name, one symbol name , one with manufacturer, one with mfr part number and so on.
simply use the in-altium tool to convert dblib to library ( or leave it as dblib)

At home i simply use a MS access database that holds the tables. I have one schlib and one pcblib file. The access file holds the rest. Loaded like any other library.  To add parts i simply have access open and can add things to the tables on the fly. Altium detects modifications to the access files and updates live.

[T3sl4co1l]

The at-scale way to do it is a database with full description (so you can find e.g. resistor, fixed, 112k, 1%, 1/8W, 0805), which links to a single symbol and a single footprint, which has been vetted, checked carefully against not just the datasheet but also tested in production.

Component creation is not to be taken lightly here, and should be reviewed by several engineers before finalizing into the production database.  This is an onerous step, but the payoff is, once you have 99% of common parts types, you don't have to think about using any of them, just plop them in and go.  You'll be creating variants of resistors and capacitors forever, but parts within an existing family are a no-brainer.

The downside is, it's impossible to edit such a database.  Even if you make changes, it's not like they will magically push to every existing schematic.  So consistency can be a headache.

This of course doesn't affect production boners; the AVLs are separate from this (or, maybe more columns in the same database, but updated from time to time) and need to be checked and re-checked in their own process.



Personally, as my database is smaller and only used by myself, I use one common SchLib and one common PcbLib, that's it.  I keep generic parts generic in the library, and set their value and part number on the schematic instead.  I put part numbers in for specific items (ICs for example) that I won't have any reason to change later on the schematic.  This tends to cause more repeated operations (setting part numbers), or copying from existing schematics (if I happen to remember using a particular value and part elsewhere), which isn't a big deal as the time spent doing that is rolled into shopping for prototype parts anyway (basically, I don't need to use a particular resistor until I've purchased it).  Clearly this is a less production-oriented approach, and that's fine as most of my customers expect to do production and maintenance themselves.

Tim

[free_electron]

The downside is, it's impossible to edit such a database.  Even if you make changes, it's not like they will magically push to every existing schematic. 

You don;t want an automatic push as that can have unexpected side-effects.
However , you do want a checker tool. Altium has that: Item manager.
This will crosscheck your design with your libraries and tell you what has changed. you then accept/reject and the ECO takes care of the rest.

If you have a vault : even more power.

[thmjpr]

The issue here is another. To avoid mistaking the component, you should identify your components by the full manufacturer part number.
Example: AD8605 vs AD8605ARTZ

...

Similarly, packages are not equal. MSSOP for example are provided in various width by different manufacturers.

Yes thats totally valid and good points.
It still relies on manual checking and getting it right up front. To see the letters "ARTZ" and know what package that should be is not so realistic, so you either have to add that as a parameter or dig down and look at the linked footprint name.

1 part = 1 symbol + 1 footprint + same footprint [manufacturer(s)+ordercode(s) ]

i have in my library the following parts:
LM324-DIL
LM324-TSSOP
LM324-SO
LM324-SON3x2

in my schematic library there is
IC-GENERIC-QUAD_OPAMP_LM324STYLE  (used for all parts , except the SON body since that has an extra pin)
IC-GENERIC-QUAD_OPAMP_LM324STYLE-15PIN (SON flavor with extra pin

In my pcb library there is
DIL14
SO127P490-14N   (SO Package 1.27mm pin pitch , 4.9mm toe-to-toe, 14 pins)
SO65P310-14N     (SO Package 0.65mm pin pitch , 3.1mm toe-to-toe, 14 pins)
SON50P300x200-14-T150x200 (SON package 0.5mm pitch, body 3.0x2.0 mm 14 pin , thermal pad 1.5 by 2mm)

Whatever i drop on the schematic will have correct information attached. the footprint, symbols and manufacturer/manufacturer order codes will be correct.

Set it up right in your library, once , and you never need to worry about it.

Same for resistors.
Simply make those with a unique footprint attached. I encode the footprint hard in the symbol.

Make a spreadsheet with the data
1 column value, one column wattage, one column tolerance, one footprint name, one symbol name , one with manufacturer, one with mfr part number and so on.
simply use the in-altium tool to convert dblib to library ( or leave it as dblib)

At home i simply use a MS access database that holds the tables. I have one schlib and one pcblib file. The access file holds the rest. Loaded like any other library.  To add parts i simply have access open and can add things to the tables on the fly. Altium detects modifications to the access files and updates live.

This is the best solution for sure, thanks for the suggestions.
I do use the library you've posted on your site although its some years old now. A few schematic parts do have the footprint as part of the name, which is nice.

At some point I'll go through and create new footprints. Its just so annoyingly simple to click on a cap and change the size, but long term for 'pro' use it doesn't make sense.

[justanothername]

add a new Parameter to the component like:
MyFootprint = CurrentFootprint
Set the Parameter to visible.
You can do this in batch with the parameter manager

[thmjpr]

add a new Parameter to the component like:
MyFootprint = CurrentFootprint
Set the Parameter to visible.
You can do this in batch with the parameter manager

Hey that worked! Thank you
edit: you can even change the font and color of it to differentiate it easily.