Low Cost PCB's Low Cost Components

Author Topic: replacing parts  (Read 1342 times)

0 Members and 1 Guest are viewing this topic.

Offline Simon

  • Global Moderator
  • *****
  • Posts: 10630
  • Country: gb
  • Did that just blow up? No? might work after all !!
    • Sparky Lab's
replacing parts
« on: July 09, 2017, 05:12:59 AM »
If say I decide I want to change a resistor value in my project, can that be done without deleting the part from the schematic and hand wiring in a new one ? so say I have already got to the PCB stage and made a prototype and find I need to change a value, a way of swapping a part with the same footprint with a same part but different value would be ideal.
The µCurrent has landed in Europe and now also selling Probe Master probes: http://www.simonselectronics.co.uk New stock now in.
 

Offline Joel_l

  • Regular Contributor
  • *
  • Posts: 146
  • Country: us
Re: replacing parts
« Reply #1 on: July 09, 2017, 06:21:06 AM »
The two ways that work for me are to just double click on it to bring up the properties window or right click on it and select properties. It seems to be picky about exactly where the cursor is when you right click or double click.

Right clicking or double clicking on the component body brings up the more complete properties window ( look in the parameters pane ). Right clicking or double clicking on the value text brings up a more abbreviated properties window. Both let you change the value.

Joel

If say I decide I want to change a resistor value in my project, can that be done without deleting the part from the schematic and hand wiring in a new one ? so say I have already got to the PCB stage and made a prototype and find I need to change a value, a way of swapping a part with the same footprint with a same part but different value would be ideal.
 

Offline Simon

  • Global Moderator
  • *****
  • Posts: 10630
  • Country: gb
  • Did that just blow up? No? might work after all !!
    • Sparky Lab's
Re: replacing parts
« Reply #2 on: July 10, 2017, 09:41:22 PM »
This does not help really, yes I could change the part numbers I suppose but I was hoping to swap with existing library parts to ensure I kept the BOM up to date and don't screw up the PCB is one is already layed out. I suppose Your suggestion would work as a last resort.
The µCurrent has landed in Europe and now also selling Probe Master probes: http://www.simonselectronics.co.uk New stock now in.
 

Offline evb149

  • Super Contributor
  • ***
  • Posts: 1568
  • Country: us
Re: replacing parts
« Reply #3 on: July 10, 2017, 11:35:00 PM »
I didn't notice a way to do this in CS. In full AD I recall there was a way in the schematic editor to right click (or something) on a component (maybe available in the properties dialog) and get a "Choose" option which would let you browse libraries and choose a different part from one of the libraries to replace the particular selected component.  As I recall it would keep certain information about the component (probably the reference designator and unique ID) so that the replacement component would just appear in the schematic in the place of the old one and it would not affect the netlist / PCB assuming the footprints and pins actually matched.

I don't see an analogous way to do it in CS when a component is already placed in the schematic / PCB and you just want to change to a different schematic library component reference with the same footprint / pinout.

I suppose there should be a way to select the part actually placed in the design based on the "variants" system to achieve the result.  But if you just want to change the base nominal component schematic library item among a set of otherwise compatible items (like different resistor values in the same package) I'm also not sure what the easiest way to do that is in CS.

I can say when you just place the desired new component on the schematic and delete the old component you can probably get OK results with just keeping either or both the old component's reference designator or maybe "unique ID" value to assign to the new component since those should be ways that the component can be matched to be "the same one" as previously existed in your netlist / PCB with minimal reassignment problems.  The potential problem you can run into with this other than the inconvenience of the mechanism is that you may end up with a flipped pinout for non-polarized resistors or whatever that you might accidentally place with a different net to pin number assignment when doing the manual replacement.  In that case you'd have to pin swap it by one means or another to make everything right with the netlist.

In short there should be an easy way to do this in CS so you can switch among different compatible library instances of, say, resistors or capacitors in the design at design time.

I imagine there is an analogous problem when wanting to select different "supplier" components from the content valult.  Maybe the content vault system gives you different / additional ways to accomplish this process since it should be a common operation to say switch from model X / distributor Y of a given component to another supply option which should still keep your netlist / footprint but change all the "parameters" as needed and hopefully also offer to preserve any of your unique adjustments to the old component (parameters or whatevever).


 

Offline Simon

  • Global Moderator
  • *****
  • Posts: 10630
  • Country: gb
  • Did that just blow up? No? might work after all !!
    • Sparky Lab's
Re: replacing parts
« Reply #4 on: July 11, 2017, 05:01:34 PM »
The content vault is a waste of time as contrary to what is infered by the name it has very little content.

On element14 they say it's possible but I'm not sure if they are talking about AD rather than CS. I also wondered if keeping the unique ID would make it work.
The µCurrent has landed in Europe and now also selling Probe Master probes: http://www.simonselectronics.co.uk New stock now in.
 

Offline ahbushnell

  • Regular Contributor
  • *
  • Posts: 72
  • Country: us
Re: replacing parts
« Reply #5 on: July 12, 2017, 04:44:12 AM »
The content vault is a waste of time as contrary to what is infered by the name it has very little content.

On element14 they say it's possible but I'm not sure if they are talking about AD rather than CS. I also wondered if keeping the unique ID would make it work.
The vault works for me.  I have been able to find parts and move to a local library.  It could be easier to do but not to bad.
 

Offline Simon

  • Global Moderator
  • *****
  • Posts: 10630
  • Country: gb
  • Did that just blow up? No? might work after all !!
    • Sparky Lab's
Re: replacing parts
« Reply #6 on: July 12, 2017, 05:00:34 AM »
I've struggled to find stuff, often only one of a whole range is available, it's like it was created by one person that only put in the parts they happened to use. The altium libraries are as bad. I downloaded the samtec headers one, it just happens to have random parts in it but not the whole range of part numbers, so they have the standard 0.1 pitch 10 pin header but not the 3 pin in the same range. If they are that patchy I can just do my own library's with the part I use.
The µCurrent has landed in Europe and now also selling Probe Master probes: http://www.simonselectronics.co.uk New stock now in.
 

Offline evb149

  • Super Contributor
  • ***
  • Posts: 1568
  • Country: us
Re: replacing parts
« Reply #7 on: July 12, 2017, 09:36:32 AM »
I haven't used the free content vault at all yet on CS and did not use it heavily with full Designer.
With "Designer" sometimes I would look for a particular specialized (as in not just a generic resistor / capacitor or such)  part like a particular IC and maybe 90%+ of the time it would not exist as a schematic symbol or as a footprint.

And when such components did exist in the vault (in my past experience) usually I didn't like the design style of the schematic symbol, it certainly wouldn't match the local standards for form and parameters, and by the time I could verify and adjust the footprint to match local standards I usually would have been better off creating it myself and been sure of my own work (or at least know who to blame).

One problem I consider "fundamental" in Altium Designer and also CS and also every other PCB CAD package I have used is that they're *so* strictly focused on ECAD that they are darn near useless at even the most fundamentally necessary and trivial aspects of MCAD or let's call it  "library science".

For instance in Designer you could use the IPC footprint wizard and easily create something sort of close to an acceptable footprint pretty quickly parametrically for certain well supported classes of packages based on the data you enter for MCAD package dimensions and tolerances and so on.  If you were REALLY careful entering those MCAD package parameters and Designer well supported the package "type" you were creating, you'd get the about the right result.   But once you clicked "OK" in the footprint wizard all that information about the parameters that were used to DERIVE the footprint were GONE FOREVER.  Then you'd just be left with lots of pads and lines and such.

So while in the "wizard" it was "easy" to verify the correctness of the driving MCAD GDT parameters that controlled the footprint's creation.  Once the footprint was in the library you'd have basically something close to worse than useless in terms of actual information about the footprint.  If you were tasked with a layout / library review and had to verify a footprint someone else created by some semi-automatic or manual process, you'd invariably end up spending WAY more time verifying the 3rd party created footprint than the time it would take to create it.

Why?  Because not having decent utilization or support of basic MCAD features you'd be left with the only tools you had to check the dimensions.  Looking at "properties" for all the pads.  Using the measuring tool point to point and point to point across numerous chords of the part / pads / boundaries to verify the dimensions.  Pulling out a spreadsheet or something to do your own relative dimensional calculation tallies of "outer edge to outer edge X and Y", "inner edge to inner edge X and Y", pad size, center to center X and Y distances, outer edges X/Y absolute coordinates, inner edge X/Y absolute coordinates etc. etc. etc. until everything could be reverse engineered BACK to the datasheet package drawing's specified control dimensions and tolerances.  WAY too much work.

Now if they'd implement even the slightest sane MCAD use and support in Altium (and other CAD vendor) products you'd have something like constructive solid geometry, parametric mechanical modelling, and geometric dimensioning and tolerancing basics supported.  So you could just glance at the "control" dimensions and tolerances of the various controlled points / lines / etc. it would be basically immediately obvious whether the GDT MCAD of the footprint matched the GDT MCAD of the datasheet at least if the datasheet drawing was any good.  And of course you'd be able to switch "with a click" to any different relative origin so you could compare different offsets etc. and get both relative and absolute dimensioning showing up.

When you'd GENERATE a foot print it'd KEEP all the relevant guide / grid / dimension / tolerance / boundary data (or rederive it on demand where possible) associated with the footprint so you could check it any time for review, DFM, whatever.

Anyway all that said about the unfortunate reality of using 3rd party footprints based on a bad MCAD UX / UI in Altium (et. al.) CAD, I'd be pretty happy if they'd just have included some more STATIC (not cloud / vault) libraries of the most common IPC compliant SMD resistor / capacitor / diode / transistor and maybe QFN / SOIC / SSOP  footprints and an easy way to "instantiate" a specific part based on a given standard library symbol and IPC footprint template.  That would make basic use MUCH easier.

Also they should have a "parameter template" system where you can define local standard parameter sets and component classes and easily apply those local standard selected parameters to new or downloaded components.  Also there should be a "parameter manager" that can work across all parts in a design though even Designer's really wasn't that good in that area to be honest, but much better than the "nothing" in CS.

Even in full "Designer" the UI to actually find / select parts from the "Content Vault" was horrid when I used it.  Maybe it has improved. 

I've struggled to find stuff, often only one of a whole range is available, it's like it was created by one person that only put in the parts they happened to use. The altium libraries are as bad. I downloaded the samtec headers one, it just happens to have random parts in it but not the whole range of part numbers, so they have the standard 0.1 pitch 10 pin header but not the 3 pin in the same range. If they are that patchy I can just do my own library's with the part I use.
 

Offline electrolust

  • Supporter
  • ****
  • Posts: 372
  • Country: us
Re: replacing parts
« Reply #8 on: July 12, 2017, 05:16:45 PM »
I didn't notice a way to do this in CS.

Wait, you can't just drop the replacement part right on top of the old part?  I've only played with CS for a few hours but I'd swear I did just that.
 

Offline electrolust

  • Supporter
  • ****
  • Posts: 372
  • Country: us
Re: replacing parts
« Reply #9 on: July 12, 2017, 05:29:38 PM »
I haven't used the free content vault at all yet on CS and did not use it heavily with full Designer.

eh?  There is no free content vault I'm aware of.  The Altium Live / designcontent thingy is a paid subscription.  It happens to come for 1 year with your purchase of CS.

Someone did post a script here on how to download the entire vault locally though.  It worked a treat for me.  Even though I have 3 yrs CS support in my particular setup it's much nicer to have the vault content locally.  [minus the fact, as Simon laments, that the content itself is spotty, dependent on manufacturer]

Quote
One problem I consider "fundamental" in Altium Designer and also CS and also every other PCB CAD package I have used is that they're *so* strictly focused on ECAD that they are darn near useless at even the most fundamentally necessary and trivial aspects of MCAD or let's call it  "library science".

... [ parametric data is not retained ] ...

Well luckily there's this easy to use program called library expert which does exactly that.  Now of course, the parameters used to construct a footprint aren't visible in your ECAD software but by naming the footprints systematically you can instantly verify the parameters by the footprint name.  Otherwise you do have to fire up the library expert tool, but the consolation is that when you switch ECAD packages you aren't a slave to their different footprint tool, you just can rely on what you did in library expert and so you gain portability.
 

Offline evb149

  • Super Contributor
  • ***
  • Posts: 1568
  • Country: us
Re: replacing parts
« Reply #10 on: July 12, 2017, 06:47:34 PM »
Oops, thanks for reminding me, I had somehow forgotten.  I lapsed into the thought the "altium content vault" was just free but that's only because you pay for it. :)   I guess that was with Designer.  Or maybe it is the same in Designer and you only get it if you are in maintenance.  Anyway thanks for the reminder about the way it works in CS.  I'll have to give it a better try to see if there's some good use case of it for me based on what is there and how one can use it.

eh?  There is no free content vault I'm aware of.  The Altium Live / designcontent thingy is a paid subscription.  It happens to come for 1 year with your purchase of CS.

Oh yeah I saw some comment mentioning that possibility but I did not at the time go looking for how / where the script is since I hadn't decided to buy CS yet.  I should find that...it sounds like a good idea at least if you can successfully modify the local items to suit your parameteric / style needs if required.  Seems like I've heard some uncertainties about that bit.
Thanks for reminding me to look for where / how to do that. 
Someone did post a script here on how to download the entire vault locally though.  It worked a treat for me.  Even though I have 3 yrs CS support in my particular setup it's much nicer to have the vault content locally.  [minus the fact, as Simon laments, that the content itself is spotty, dependent on manufacturer]


Good point, thanks.  I used to use the pcb libraries library expert thing back when I used eagle / designspark.  I haven't tried it in a while and not since I got CS.  I should consider to use it particularly since CS doesn't (IIRC) have an IPC compatible footprint generator.  I'll have to get used to the IPC naming convention moreso than I yet have.  It is as you say nice to have a systematic and descriptive naming convention.  Someone should write a program to go back and forth between the "name" and the "parameters".  Maybe library expert does that round trip, I've never thought to try / check, only noticed the systematic default generated names.  It is just a pity that what little dimensioning Altium has (grids, guides, dimensions) it doesn't actually use when it creates / displays / interprets footprints and other PCB mechanical objects.

Well luckily there's this easy to use program called library expert which does exactly that.  Now of course, the parameters used to construct a footprint aren't visible in your ECAD software but by naming the footprints systematically you can instantly verify the parameters by the footprint name.  Otherwise you do have to fire up the library expert tool, but the consolation is that when you switch ECAD packages you aren't a slave to their different footprint tool, you just can rely on what you did in library expert and so you gain portability.

 

Offline evb149

  • Super Contributor
  • ***
  • Posts: 1568
  • Country: us
Re: replacing parts
« Reply #11 on: July 12, 2017, 06:51:00 PM »
I just tried it on my existing schematic (using self-made schematic symbols and components / footprints) and all it did in the schematic anyway was to plop the new resistor schematic symbol literally on top of and electrically in parallel with the old one.  It repeated that behavior despite different ways I tried to "stack" them.. holding shift / alt / ctrl, whatever.
So if there's a swap vs. merge mode I haven't found it.  And I have no recollection of how to do that in Designer other than using what I seem to recall is the properties dialog / library -> "Choose" dialog button.

EDIT: Of course it is possible I didn't do it right or I needed to include some particular metadata in the components / symbols to make it work or they had to be Vault components or.... something.

I didn't notice a way to do this in CS.

Wait, you can't just drop the replacement part right on top of the old part?  I've only played with CS for a few hours but I'd swear I did just that.
 

Offline electrolust

  • Supporter
  • ****
  • Posts: 372
  • Country: us
Re: replacing parts
« Reply #12 on: July 12, 2017, 07:41:39 PM »
I just tried it on my existing schematic (using self-made schematic symbols and components / footprints) and all it did in the schematic anyway was to plop the new resistor schematic symbol literally on top of and electrically in parallel with the old one.

Thanks for confirming.  ugh how awful!  Guess that's the final nail in the CS coffin for me.  I'll revisit when 1.5 comes out.
 

Offline tarribred61

  • Contributor
  • Posts: 10
  • Country: us
Re: replacing parts
« Reply #13 on: July 13, 2017, 02:57:44 AM »
You can place in the replacement component as a new part near the old one and then renumber the designator to match.  If it uses the same footprint it should match up.  There is actually a unique ID field in both schematic and PCB instances that are used to synchronize them.  You can manually copy the unique ID from the old schematic part to the new one but it may not be necessary as it will fall back to use the designator.

 

Offline evb149

  • Super Contributor
  • ***
  • Posts: 1568
  • Country: us
Re: replacing parts
« Reply #14 on: July 13, 2017, 03:11:53 AM »
Yes that works, I have done it that way. But you also must have the pin number to net connections the same as I mentioned above which is obvious except for resistors or unpolarized components where the symbol may not normally be created to even show the pin numbers so it is an added inconvenience.
But a pretty slow / inconvenient process for which there should be a "point and click" solution.
Maybe the "variant" editor scheme will let you freely choose among such alternatives, but that's kind of inelegant when a variant is not what you're actually creating.

You can place in the replacement component as a new part near the old one and then renumber the designator to match.  If it uses the same footprint it should match up.  There is actually a unique ID field in both schematic and PCB instances that are used to synchronize them.  You can manually copy the unique ID from the old schematic part to the new one but it may not be necessary as it will fall back to use the designator.
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf