On 03:35 PM 11/05/2001 -0700, Abd ul-Rahman Lomax said:
>At 11:45 AM 5/11/01 -0700, Rimas Avizienis wrote:
>
>>if i have a circuit replicated eight times in a design, is there an easy
>>way to do the layout for one circuit and then replicate the layout for
>>the others?
>
>Glad you asked.
>
>It would be nice if we had some artificial intelligence that would
>recognise replicated circuit blocks at the schematic level, regardless of
>how the individual components were labelled, and it would then take a
>physical layout of one block and replicate it, assigning the correct
>reference designators. But we don't have that, at least not in Protel, not yet.
>
>When a PCB block is copied, there is some control over how the designators
>are copied. See Paste Special/Paste Array. This will give designators a
>fixed increment, and if the schematic has been drawn such that the
>reference designators have the same increment between the blocks, you are
>practically home free. But we don't always have this luxury, and it makes
>for reference designators with lots of gaps in the numbering.
>
>Now, I'm just finishing up a board with 8 identical blocks. I had drawn
>the schematic, and the eight blocks existed on two sheets of the
>schematic, 4 per sheet. In some ways, it would have been a little easier
>if there had been one block per sheet. It was auto-annotated, see below
>for a comment about that.
>
>I then designed one block, working with the components until I had an
>efficient placement (this needed to be designed at almost 100% density);
>it was long and skinny. I then made gerbers of this block, of the
>silkscreen and padmaster layers, and imported them to an otherwise unused
>mech layer, I'll call it the placement layer. I stepped seven copies of
>this placement layer in a row adjacent to the original. I made sure that
>the full array would fit on the PCB before I went any further.
>
>I made a list of which parts in each block corresponded to the parts in
>the first section. This was easy because the increment for each type of
>component was equal to the number of that type of component (C, R, etc) in
>the array. I had been careful to arrange the schematic in the first place
>so that the numbering would occur in this way (this has to do with the
>sequence in which parts are placed as well as the annotation command
>setup). Had I not done this, it would have been only a little more
>difficult. In any case, if you make a mistake here, it will self-correct
>since it will create DRC errors.
Could you not use the Tools|Place From File... function after having
created a suitable place file? Creating this file from a spreadsheet
couldn't be hard? Place the first block. Export the pik
file. Copy/paste/clip/massage etc until you have the other blocks with the
desired offset and then run this file back through the place from file
function. This could well be quicker especially if you have good component
designators that allow simple editing in the spreadsheet. Hasn't someone
discussed this feature before in doing multi-channel work? This is the
sort of thing you like doing, Abd ul-Rahman, is it not - mucking about with
text files. I'll leave it to the reader to think about how doing the
placement of the multi-channels in a separate PCB and copying and pasting
back might make the creation of the place file easier (or at least an
easier to work with pik file exported from the
I also think that there was an add-on from someone that was designed to
help multi-channel work but it may only have been to assist component
designator numbering.
It would be worth some investigation and a decent clear tutorial on the
matter - possibly an HTML page(s) complete with graphics and file snippets
showing how the changes can be done. Anyone offering? I would but my
Protel Assoc hours are busy elsewhere at the moment.
Protel CSC could even do something like this and post it in there tutorial
section of their www site.
Ian Wilson
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/subscrib.html
* - or email -
* mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Browse or Search previous postings:
* http://www.mail-archive.com/[email protected]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
