SMT manual placing: a thougt silk screen use component value not name/ref

[Kjelt]

Hi, just a quick thought.

Up till now I always used for the silk screen the component reference name so R1, R2 etc. you always see this.
But actually when manually placing the SMT components this is a PITA.
Before every placement you have to look at your cheat sheet which reference is the same value and where it is located.

So I thought why not use the component value at the silk screen and save a lot of time during placing?
Yeah I know if something is broke later on or you have to change some component you have to lookup where it is located, but still this happens so rarely I rather save the time during placing.

Like to hear your thoughts, and keep it to manually SMT placing, I can understand that if you have a P&P or do 100 boards a day you have different requirements.

[ConKbot]

If you have the space, go for it!  Especially for manual placement, if you can fit it on the PCB, it'll help. Its just that if you have 5-6 0402's in close proximity, your silkscreen will be taking up way more space then your parts, but not everything has to be high density.  Looking at 2 places (board/parts) will be a lot faster than looking at 3 places. 

If your pcb is too dense, then go for putting it on the assembly drawing instead, so you have a graphical index, rather than a table to look up parts.

[Alex Eisenhut]

Who has the space for that? And what if the values need changing after a ECO? I don't even have space for refdeses anymore!
And why call it a "cheat sheet"? It is simply the assembly drawing, there is no cheating.
You can use the color-coded flip chart drawings too.

[CatalinaWOW]

This might be an opportunity for some software vendor to add yet another layer to the design file.  A value layer intended to print on a separate (perhaps transparent) sheet would not have to avoid component footprints, vias etc. and would therefore have more room for text.  This could be useful even during the maintenance phase, when a visual inspection of the board often identifies bad components, but it is a PITA to locate the reference number in the schematic where the numbers often don't proceed orderly from top left to bottom right.

[voja]

I always wrote component value at the silk screen, and I was always told that it does not look professionally. But of course, I don't care

[Alex Eisenhut]

This might be an opportunity for some software vendor to add yet another layer to the design file.  A value layer intended to print on a separate (perhaps transparent) sheet would not have to avoid component footprints, vias etc. and would therefore have more room for text.  This could be useful even during the maintenance phase, when a visual inspection of the board often identifies bad components, but it is a PITA to locate the reference number in the schematic where the numbers often don't proceed orderly from top left to bottom right.

Something like this

http://www.unisoft-cim.com/pcbview.htm



I used to make these drawings by hand, layer by layer in Allegro.

[pickle9000]

I don't do it myself but have seen it done many times. I have no problem with it, any system will have it's down side.

[pickle9000]

This might be an opportunity for some software vendor to add yet another layer to the design file.  A value layer intended to print on a separate (perhaps transparent) sheet would not have to avoid component footprints, vias etc. and would therefore have more room for text.  This could be useful even during the maintenance phase, when a visual inspection of the board often identifies bad components, but it is a PITA to locate the reference number in the schematic where the numbers often don't proceed orderly from top left to bottom right.

Something like this

http://www.unisoft-cim.com/pcbview.htm



I used to make these drawings by hand, layer by layer in Allegro.

Dex is probably the only program that would/could implement it. It's is a feature so probably worth an ask.   

[jolshefsky]

If you have a low count of unique values (e.g. 5 or 10) you could make your reference designators coded to the value. For instance, RA100 to RA134 are all 1K, RB100 to RB108 are 10K, etc. It would also be easy to visually check on a BOM sorted by part number since all the values would clump together.

[Alex Eisenhut]

I'm probably not being super clear here, but the flipchart concept is that you have a list of, say, 8 part numbers per page, color-coded, and the locations are highlighted. Then when you're done with those parts, you flip to the next page and the next set is highlighted.
The color highlighting in Allegro made this simple enough, a script would highlight each p/n on the design, but I stitched the PDF together manually.
There was a program that did everything automatically but I can't find it anymore.
Of course we are talking maybe a hundred or so part numbers and maybe 200 parts per board, nothing big.

[ajb]

This might be an opportunity for some software vendor to add yet another layer to the design file.  A value layer intended to print on a separate (perhaps transparent) sheet would not have to avoid component footprints, vias etc. and would therefore have more room for text.  This could be useful even during the maintenance phase, when a visual inspection of the board often identifies bad components, but it is a PITA to locate the reference number in the schematic where the numbers often don't proceed orderly from top left to bottom right.

Something like this

http://www.unisoft-cim.com/pcbview.htm



I used to make these drawings by hand, layer by layer in Allegro.

Dex is probably the only program that would/could implement it. It's is a feature so probably worth an ask.

I do this in Altium all the time.  All parts have a "comment" property, which is basically just a parameter that gets special treatment, and is typically used to hold the component's value.  I have a user script that moves comments and designators to dedicated mechanical layers, and scales and centers them on the appropriate component.  Since they're on dedicated layers, I can spit them out as gerbers to send to a contract assembler, or if I'm hand assembling a prototype I'll do PDF prints of each comment/designator layer (the relevant text being dark colored, with the silkscreeen in light grey behind for orientation).  If I have a particularly dense design or long designators I'll typically need to spend a couple minutes to nudge some things this way and that to keep things from overlapping.  I'm sure you could take this further and do multiple prints with groups of values highlighted, but I haven't bothered to try figuring that out yet. 

[Kjelt]

I'm probably not being super clear here, but the flipchart concept is that you have a list of, say, 8 part numbers per page, color-coded, and the locations are highlighted. Then when you're done with those parts, you flip to the next page and the next set is highlighted.

That is what I call my cheat sheet, I print out the pcb layer and highlight with a marker the same value parts with the same colour and write down the value. Last design I had 20 A4's sheets.
But indeed I use 0603 at the moment so have the space for silkscreen but if you go down to 0402 and really have a dense populated board I can see there is no room at all anymore 

[Alex Eisenhut]

I'm probably not being super clear here, but the flipchart concept is that you have a list of, say, 8 part numbers per page, color-coded, and the locations are highlighted. Then when you're done with those parts, you flip to the next page and the next set is highlighted.

That is what I call my cheat sheet, I print out the pcb layer and highlight with a marker the same value parts with the same colour and write down the value. Last design I had 20 A4's sheets.
But indeed I use 0603 at the moment so have the space for silkscreen but if you go down to 0402 and really have a dense populated board I can see there is no room at all anymore 

Oh that's fantastic, so you're getting to a point where you're just like everyone else! You just need to automate this tedious task, that's all.
This is the way to go. 0603 for me is "vintage"... You are now ready to go to 0201.  Except for home projects, then 1206 is fine...

[T3sl4co1l]

There is exactly such a thing: it's called the assembly drawing output.

Usually this contains some mechanical layers which describe the centers or outlines of the components, the silkscreen (and therefore refdes, plus what the board visually looks like), and optionally, comments or other strings (as mentioned above) relating to footprint name, value/part number, etc.

I haven't seen a color coded / layer coded approach before.  Most EDA tools have a fixed number of layers, so you can't keep adding one layer for each unique part on the board.  If this were available, you could conceivably add a unique identifying layer to each unique component value in your library (so the schematic library would consist of e.g. one single resistor symbol, with hundreds of instances of values, part numbers and such; and the PCB library would be the same way, having one footprint and hundreds of instances of this customized layer or label property).

Finally, using such a tool: you could print a PDF version of the BOM, and add these graphical layers, which could be controlled with JavaScript; or the same thing in HTML in the browser.  The layers themselves could be printed, physically, onto transparency sheets, but this wouldn't be very effective for BOMs over 20 or so (the transparencies simply aren't *that* transparent, enough that you can still see through a thick stack of them!).  Or they can be printed onto plain paper, one or a few layers at a time, with a legend, which would probably be the best physical approach.

Not sure if that's quite related to what you had in mind, but it's an interesting thought to entertain.  Maybe not the most useful compared to other tools or methods (like, a PnP machine ), but definitely within the realm of possibility in one of these EDA tools.

Tim

[c4757p]

And why call it a "cheat sheet"? It is simply the assembly drawing, there is no cheating.

"Cheat sheet" is a common colloquialism for any quick reference sheet

[pickle9000]

This might be an opportunity for some software vendor to add yet another layer to the design file.  A value layer intended to print on a separate (perhaps transparent) sheet would not have to avoid component footprints, vias etc. and would therefore have more room for text.  This could be useful even during the maintenance phase, when a visual inspection of the board often identifies bad components, but it is a PITA to locate the reference number in the schematic where the numbers often don't proceed orderly from top left to bottom right.

Something like this

http://www.unisoft-cim.com/pcbview.htm



I used to make these drawings by hand, layer by layer in Allegro.

Dex is probably the only program that would/could implement it. It's is a feature so probably worth an ask.

I do this in Altium all the time.  All parts have a "comment" property, which is basically just a parameter that gets special treatment, and is typically used to hold the component's value.  I have a user script that moves comments and designators to dedicated mechanical layers, and scales and centers them on the appropriate component.  Since they're on dedicated layers, I can spit them out as gerbers to send to a contract assembler, or if I'm hand assembling a prototype I'll do PDF prints of each comment/designator layer (the relevant text being dark colored, with the silkscreeen in light grey behind for orientation).  If I have a particularly dense design or long designators I'll typically need to spend a couple minutes to nudge some things this way and that to keep things from overlapping.  I'm sure you could take this further and do multiple prints with groups of values highlighted, but I haven't bothered to try figuring that out yet.

I was thinking more along the line of simply a layer that shows values. No editing required. Couple clicks to do the entire project or revert back.

[Alex Eisenhut]

And why call it a "cheat sheet"? It is simply the assembly drawing, there is no cheating.

"Cheat sheet" is a common colloquialism for any quick reference sheet

Fair enough, I always took it to mean some sort of home-made thing to make up for a lack of proper documentation.

[kjs]

I was thinking more along the line of simply a layer that shows values. No editing required. Couple clicks to do the entire project or revert back.

That's what I use in Eagle all the time. Turn off all other unwanted layers and keep the value layer is on. Someone at my place wrote a script where you can even highlight all identical values at the same time and step through.

[JuKu]

But actually when manually placing the SMT components this is a PITA.

Indeed. And it gets worse when the board is tight and you don't have room for designators. When I did placement manually, I used several tricks to make it easier. I use Altium, which makes these easy:

-Printouts that have the designators on the components.
-Printouts that have the values on the components
-Printouts that have certain components highlighted (such as a shee that shows all bypass caps)

For a complex board I used to have ten or twenty sheets. It helped, a lot. From Mike here I learned to use sheets pf cardboard and have part strips attached to them with double side tape. This is good for two reasons: It is easier to rotate the component sheet than the board and that keeps your "board mental navigator" on the map. Secondly, when you put the components on such board, you put there as many as there are on the board. This way, you get to put down all parts of a certain value without missing any.

These help, a lot, but I still ended up building a machine.

[mikeselectricstuff]

As mentioned the problem is what happens if you need to change a value
However you can probably solve it for a large proportion of non-critical parts like pullups, decoupling etc. by marking those, maybe with just a letter, so you only need to look up what's left.
Similarly if you have a lot of parts that are all the same value, and if they change they will still be the same, either mark with a single letter, or use a different refdes prefix.