PCB Layouts

[SBHarwin]

Hello,

I am an apprentice Product Design Engineer for Harwin and I've been given a task, that I'm hoping the people in this forum can help me with.

I'm looking into how Harwin can supply PCB schematics/layouts for our connectors, and the preferred format/file types and programmes for anyone looking to use them.

Can anyone help me identify which schematic formats/file types are most commonly used, and what programmes are the best to make library layouts?  Are there any generic formats/file types which import well into the majority of PCB schematic programmes?  What programmes are easy to use?  Any and all recommendations gratefully received!

Thank you!

[enz]

Hi Sam,

nice to see that a manufacturer cares about this topic.

To be honest, i always do schematic symbols and footprints myself. For me there is no need for a manufacturer supplied file.

BUT: I really care about 3D-step files. I only use connectors from manufacturers that supply 3D step models on their website, of course without the need for cumbersome registration or something like that. For me the use of step models in the layout program (Altium Designer in my case) is essential to check the mechanical parameters of the design.

Good in supplying step models are, for example, TE, Molex and WAGO. Would be very nice, if Harwin would do the same.

[Rufus]

I'm looking into how Harwin can supply PCB schematics/layouts for our connectors, and the preferred format/file types and programmes for anyone looking to use them.

The preferred format would be that of the CAD package the particular customer is using. There are no standard formats and conversion between formats is generally down to the package you are using being able to import them usually with less than perfect results.

If you look here http://www.pcblibraries.com/FPX/ you will see a list of CAD packages a company trying to provide generic libraries supports.

To be honest IMO there isn't great benefit in you trying to provide CAD symbols and footprints. A lot of companies simply would not trust or use them. There are also style considerations which affect schematic symbols and manufacturing process variables which affect footprint requirements.

I do think there is benefit in providing accurate 3D models and complete and accurate drawings. In the past I have needed a physical part and pair of callipers in my hands to be able to create a footprint far too often because drawings were lacking. 

This http://www.accelerated-designs.com/ultra-librarian/ is another site to check. I think some companies have struck a deal with them to distribute a limited version of their product with libraries for that company. Not suggesting it is a good idea - from the little I looked at it the results were too horrid to use.

[free_electron]

Step files and or gerber data. I prefer step files. Samtec supplies step for everything they have.
The advantage of step is that you can do more than just pcb. You can do the mechanical assembly as well.

[SBHarwin]

On the Harwin website we provide both step and iges files for almost all of our products! 
Enz, we do have a quick registration process for the CAD download, however, I've signed up myself and found it not to be too cumbersome.

Thanks for the feedback guys, interesting to find out just how useful step files and that people tend to do their own footprints! Does anyone else have any experience of using existing footprint libraries?

[poorchava]

Existing libraries are useful when dealing with multi-pin semiconductors. For example I would really look hard for existing library if I had to draw a 1000-pin BGA symbol/footprint. On the other hand few days ago I have drawn a 100-pin STM32F4 symbol and it took me like 15 minutes.

And connectors are much more straightforward, since pins do not have specific functions (gnd, vdd, ports, etc). So creating a symbol for 200-pin connector could take 10 minutes or so. Footprints can be generated automatically to a large degree. I think those are the reasons why people tend to draw them on their own.

I have used existing libraries for stuff like microcontrollers, fpgas, memories, basically anything that has many pins, although that's only when I can get those easily.


Here's a timelapse of creating schematic symbol for 100-pin component (quality sux though, encoding issues)

[komet]

I always do my own footprints and what I would appreciate would be if dimensional drawings of the recommended layout would display the centre rather than the outside position of the pads, and referenced from the centre of the part, because that is what one puts into the PCB layout tool.

The other day I did this Harwin part:

http://www.harwin.com/include/downloads/drawings/M80-828.PDF

In order to input it, I had to do the following calculations:

X-position of pads: 2.0mm * (n + 1/2)
Y-position of pads: (8.0mm - 3.2mm) / 2 = 2.4mm
X-position of mounting holes: (2.0mm * (number of pins per row - 1) / 2) + 2.25mm = 7.25mm for the 6x2 pin part
Y-position of mounting holes: 2.38mm, the only value explicitly stated on the datasheet

It would have been nice to have these values on the datasheet to start with.

[metalphreak]

If you do Eagle parts, check out this: http://devbisme.webfactional.com/content/taking-ahg-out-making-parts-eagle

[Psi]

+1 for supplying 3D Step models of the component.

[nctnico]

I always do my own footprints and what I would appreciate would be if dimensional drawings of the recommended layout would display the centre rather than the outside position of the pads, and referenced from the centre of the part, because that is what one puts into the PCB layout tool.

It would have been nice to have these values on the datasheet to start with.

I couldn't agree more! For some reason some mechanical drawings are real puzzles.

[c4757p]

I always do my own footprints and what I would appreciate would be if dimensional drawings of the recommended layout would display the centre rather than the outside position of the pads, and referenced from the centre of the part, because that is what one puts into the PCB layout tool.

It would have been nice to have these values on the datasheet to start with.

I couldn't agree more! For some reason some mechanical drawings are real puzzles.

+1 I've yet to see a land pattern drawing that was drawn by somebody who's ever had to enter one into PCB software.

[SBHarwin]

I always do my own footprints and what I would appreciate would be if dimensional drawings of the recommended layout would display the centre rather than the outside position of the pads, and referenced from the centre of the part, because that is what one puts into the PCB layout tool.

It would have been nice to have these values on the datasheet to start with.

This is very interesting to learn and it seems as if it's a common issue! I will definitely look into how we can try and improve and solve this customer issue on our drawings at Harwin.

And connectors are much more straightforward, since pins do not have specific functions (gnd, vdd, ports, etc). So creating a symbol for 200-pin connector could take 10 minutes or so. Footprints can be generated automatically to a large degree. I think those are the reasons why people tend to draw them on their own.

I have used existing libraries for stuff like microcontrollers, fpgas, memories, basically anything that has many pins, although that's only when I can get those easily.

Thanks for all the information!


We try to keep our layouts fairly simple so that it's easier for customers to produce their own, however, if there is any way in which extra assistance could be provided by ourselves to make the process nicer and easier for customers then please advise! Such as a library of layouts etc.

[mamalala]

Enz, we do have a quick registration process for the CAD download, however, I've signed up myself and found it not to be too cumbersome.

This is what i don't understand. Why require a registration for that? What are the companies doing with that data? After all, they want it, so they surely want to use it in some way. If they don't want to use it, why require the user to give it away in the first place?

Keep in mind that there are security issues involved as well. You simply can not guarantee that this data is safe. Believing otherwise is worse than foolish.

Really, it would be great if companies would stop that silly practice and simply put a download link to these files somewhere and be done with it. Makes it much easier and safer for the user, and it also makes life easier for you guys since you don't have to maintain those datasets anymore.

Whenever i come across a site that requires me to register to download some CAD files for their products, i enter bogus data. If that is not possible because of some confirmation eMail crap, i simply stop at that point and look for alternatives that don't want to grab my personal information, read: some competing company. It's that simple.

Greetings,

Chris

[Rufus]

Enz, we do have a quick registration process for the CAD download, however, I've signed up myself and found it not to be too cumbersome.

This is what i don't understand. Why require a registration for that?

I completely agree. They are not preventing anyone they don't want to have the information from getting it. They are not getting any useful legal protection for the information - they are just making things a pain in the arse for everyone.

Imagine walking into a shop and asking to look at something and the assistant brings out a form to fill in, takes your mobile phone number and calls you on it to prove you gave a real number. I would tell them to use the form as a suppository and walk away.

Be careful, I hear an Elf that works for Santa just registered on your site and is going to steal all your IP...

[AndyC_772]

I agree with many of the above comments, they're worth re-iterating:

- if a company insists I register just to get technical data on an off-the-shelf component, I go elsewhere. I only come back to that company's site as an absolute last resort if I can't find a competitive product that does the same job. Seriously, if I need to contact you then I will do - honest! -and if I can get all the data I need from your web site, then I'll design in your part and you'll get a purchase order in due course from my CEM. Just please bear in mind that sometimes I just want to buy a connector, not necessarily start up a long-term business relationship.

- schematic symbols for connectors are pretty easy to draw, and everyone has their own personal style - not to mention needing to add their own part numbers and other metadata. I wouldn't really be inclined to bother producing them at all - but if you do, Orcad is the format used by most of the companies I've worked for.

- PCB symbols are more useful, though even then, there's a lot of 'house style' features which you'd never get right for everybody. Instead, make sure your mechanical drawings are complete, fully dimensioned, and be sure to include the dimensions that someone drawing the symbol would actually need: the dimensions of each pad, the distance from the drawing origin to the centre of each pad, and ensure that both the pins and the mechanical (silkscreen) outline of the part are dimensioned from the same origin.

- 3D solid models are definitely useful

[mamalala]

... the dimensions of each pad, the distance from the drawing origin to the centre of each pad ...

And make sure that the origin is what a pick&place would use, or at least the center of the part itself. The origin being in the lower-left, for example, is of little use....

Greetings,

Chris

[free_electron]

... the dimensions of each pad, the distance from the drawing origin to the centre of each pad ...

And make sure that the origin is what a pick&place would use, or at least the center of the part itself. The origin being in the lower-left, for example, is of little use....

Greetings,

Chris

NO ! the origin should be a corner pin . Any cad tool worth its salt will calculate the pick and place origins itself based on the center of the crossing diagonals. ( which is how the pick and place robots do it. this is standard in the industry )

The reason for have the 0:0 coordinate laying on a pin is that you simple define a drawing grid that is a multiple of the pitch and with an array past you have the footprint in a few clicks. if you need to go and recalculate all that crap it becomes error prone.

If you are going to make datahsheets for the connector please used the JEDEC nomenclature. there are definitions for dimension like e, E d,D B1, B2 etc ... most  serious cad programs have wizard tht follow the jedec standard. simply punch in the numbers according to the standard and the footprint rolls out ,exactly correct. Combine that with a STEP model and you are golden.

Right now I am doing a very complex boardset that needs to stackup in 3 dimensions ( horizontal board with side connector connecting to an add-on. the big board has a vertical riser with 3 plugins , 2 of which that also mate horizontally while the third mates with the plugin. I need to work out all connector placements , length of the standoffs, position of the screws, guide rails for the rack. without STEP files this is a friggin nightmare.

Now I just plonk down the parts , export each individual board as a completed STEP file and load those as completed entities in the main project. In 3D space I can manipulate each sub board , including all it parts and see that the connectors line up , the heat sinks line up , tall capacitors on a sub assembly don't impeded other parts on an underlying board etc... I've kicked out multiple suppliers during this design simply because they have no accurate step files.
for capacitors and the like I make em ( that's just a cylinder ) but for a 204 pin samtec board to board connector ... I want the damn model (which samtec happily provides. they have models for almost anything. and the missing ones take about 2 hours to get them emailed to me from their cad department.

there is no excuse these days for not having STEP files. everyone in the component business is on Solidworks, Catia, ProEngineer or other real 3D kernel software anyway. and all that software can spit out STEP files with 1 mouseclick.

[mamalala]

... the dimensions of each pad, the distance from the drawing origin to the centre of each pad ...

And make sure that the origin is what a pick&place would use, or at least the center of the part itself. The origin being in the lower-left, for example, is of little use....

Greetings,

Chris

NO ! the origin should be a corner pin . Any cad tool worth its salt will calculate the pick and place origins itself based on the center of the crossing diagonals. ( which is how the pick and place robots do it. this is standard in the industry )

Uhm, and where is the difference to what i proposed? For any random part, the crossing diagonals would be the center of the part. However, there can be parts where the part's center is not the best option to use. Imagine a connector that goes beyond the PCB dimension by more than a half of it's size. In such a case it might be beneficial to have the p&p center onto the PCB side instead of "mid air".

Admittedly i know little about p&p machines, but that's how i imagine things should be, derived from a hell lot of time spent manually populating boards. The center of the part might not always be the best place to put it down.... But i'm more than happy to be corrected on that based on facts.

Greetings,

Chris

[AndyC_772]

Personally I don't much care where the origin is on the drawing, it's trivial to change it as the last step once the symbol has been transcribed into the PCB software.

[gregariz]

Admittedly i know little about p&p machines, but that's how i imagine things should be, derived from a hell lot of time spent manually populating boards. The center of the part might not always be the best place to put it down.... But i'm more than happy to be corrected on that based on facts.

Thats actually pretty common. You can load in the P&P file into the machine but something like a D-Pak or something with long legs poking out one side will often be manually adjusted using something like a laser/vision locator. From what I observe, not too much faith is placed in these files. The older machines are even worse in that many jobs are completely set up manually. Ie. The operators manually locate the centers of all components on the tapes, trays, and sticks and then manually locate the corresponding footprint centers on the PCB. Then they do a dry run and make any readjustments. Setting up some of these machines can take a bit of time.

[marshallh]

I can confirm this, when I supplied my centroid file for a design to the assembly house they said some parts were off origin but it was not an issue, because they were going to fine tune the picking head offsets anyway. And the centroid data were just a guidelines to tie back to the reference designator.

[mamalala]

Just to confirm that i'm getting this right: The center of a part is quite often not really what a p&p would need, thus fine-tuning is needed? So the center-of-whatever-diagonals is just a silly leftover of "the good old days"?

If so, then hell yeah, let the manufacturers begin to put their origins in a place where p&p machines would be most happy with. As long as all the other dimensions are clearly refering to that origin, all should be fine. I mean, really, we all can do addition and substraction when we need to put all that into footprint files/libraries, right?

Greetings,

Chris

[free_electron]

No we don't want to calculate !
Set origin at pin 1. Then there is no discussion of at least where pin 1 is on the bloody damn component !
All you need then is row pitch and pin pitch. All cad tools have an array copy function. Simply tell it how many rows and how many pins per row. Set the placement grod to the given pitch and done. At this point the computer does all the stupid work like calculating. Thats what that 5000$ software is for.

For most components like resisotrs, caps and the like the centroid (crossing diagonals) is used.
A modern pick and place machine needs very little manual tuning. The have a downward camera, an upward camera and a side camera. The machine grabs the part from the feeder line ( tape, stick or bulk). As the stage moves the part is spun around 360 degrees in the horizontal plane. The machines computer can now determine width and langth ( smallest and wides surface seen while spinning) and it also knows the offset of how the part sits in the nozzle. The stage is now being x,y and theta corrected in respect to the centroid data that was delivered by the cad.

This takes milliseconds for the robot. The stage has now arrived at part coordinates and the downward looking camera has begunlooking for the pads on the board. The centroid data gave it the 'rough position' and rotation . The machine now looks for the pads draws the centroid grid itself and calculates accurate center and theta. Compensate the stage and plonk the part down. Perfect fit. Every single time.

No teach in needed. Board can sit crooked in the conveyer, parts can sit crooked in the tape. All that is needed is center coordinates. The vision system does the rest. It's always been like that and it will always be like that as it is the simplest way for the machines to do their work. All other stuff the machines do is rime optimisation , like calculating the flightpath and precompensate as much as possible. Thats where you pay the big money. If you want throughput you will pay.

The really advanced machines actually start by placing two compinents on opposite corners of a board. That way they have an overview of the overall theta ( the rotation angle ) and xy offset of the board in the conveyer.

I have posted , in another topic, how these modern machines fully self align based on a single lasermark on the machine chassis. These machines shoot 0201 and 01005 without blinking at a rate of 50k components per hour.... My subcontractor has one. Mitsubishi.

True ,there are exceptions like special connectors that may have a tab to be picked up . But that is a matter of giving a delta xy from center.

Back to the cad world : here we try to make the manual labour as easy, simple and short as possible. Gimme a corner pin , grid space and off we go. Draw the silkscreen outline around it , and let the cad software do the centroid calculation. Some cad tools let you use a mechanical layer to provide the exact picking position.  Be default you leave that as 'centroid' but you can flick the option to manual and set the pick coordinate yourself.

When the p&p data is generated everything falls into place by itself.

And follow the JEDEC standards for the parameters. Like i said : any cad tool worth its money has a wizard that uses the JEDEC naming convention. Simply plonk in the numbers fro. The datasheet and the wizard does the rest.

[free_electron]

Admittedly i know little about p&p machines, but that's how i imagine things should be, derived from a hell lot of time spent manually populating boards. The center of the part might not always be the best place to put it down.... But i'm more than happy to be corrected on that based on facts.

Greetings,

Chris

Manual popularion is completely different. If you got no experience with pick and place, don't "imagine":  all that stuff has been worked out long ago and your imagination is wrong.

As for facts : my customers build about 1 million boards a day... I know how it is done as i am involved in the entire design from the silicon specification all the way to the assembled , tested and initialized product.
When we come up with a new chip with a new package everything is looked at. From pcb routing , layout , soldering, thermal, assembly , relibility, testability  and much much more. In the end we need our end customer to deliver a product. So we partner on all aspects of the design.

[nctnico]

Just to confirm that i'm getting this right: The center of a part is quite often not really what a p&p would need, thus fine-tuning is needed? So the center-of-whatever-diagonals is just a silly leftover of "the good old days"?

If so, then hell yeah, let the manufacturers begin to put their origins in a place where p&p machines would be most happy with. As long as all the other dimensions are clearly refering to that origin, all should be fine. I mean, really, we all can do addition and substraction when we need to put all that into footprint files/libraries, right?

It depends a bit on the mechanical aspects as well. Recently I designed a circular board with about 90 LEDs along the edge. I designed a LED footprint where the centre of the component is at the base of the plastic housing. That way I could simply punch in the coordinates and rotation of the LEDs without having to calculate an offset. Same goes for connectors. On Euro cards the position of the connectors is specified by the mounting holes. If the mounting hole is the reference of the footprint you can't go wrong. OTOH there are also board-to-board connectors where you can't use holes for the reference. In those cases I use the centre of the connector so there is no chance for error in calculated offsets. If I position the connectors in the same place on both boards it will fit.