Itead brd outline, which layer?

[AlfBaz]

Itead say "Outline or shape should be included in at least one layer"
1. Does this mean one of the existing layers that they stipulate or on its own?
2. If its the former, put it on the top overlay with dimensions?
3. I'm doing a prototype for the SMPS section on a larger project. It's multi-rail and is fed from a LI-ION batter charger cct that's also included on the PCB. This thing is only going to be 2 layer but the larger project is 6 layer 2 of which are power and ground planes. I'm not sure wether to go for the largest PCB thickness they offer (without extra cost) and if it works here it will work on the final because the top layer will be closer to the plane layers thereby having better capacitive coupling, or go as thin as possible to get a better representation of what the supply will be like on the final board... Any thoughts?

[Jon Chandler]

The CAM tool for Eagle from Seeed puts the board outline on every layer.  I've been following this convention since I had a problem on one order from iTead where they couldn't find the outline which was only on one layer.

The Seeed CAM file follows the same naming convention as iTead uses and works well for iTead too.

[AlfBaz]

Thanks for the info Jon. I already sent the files and put it on the top overlay.
I'll have to read up on the cam generator, I don't know how to edit anything with it which means I would have to have the outline on all my PCB layers. Not something I think I would like...

[Jon Chandler]

The CAM processor in Eagle is pretty easy to use.  Probably easiest to start with the Gerber CAM file provided by Seeed.

Start the CAM processor and load the Eagle board file.  There will be tabs along the bottom for each Gerber layer (top copper, top silk, etc).  If you click the tab for a particular layer, on the right side of the box is a column of Eagle layers, with the ones used to generate the Gerber layer checked.  Layer 20 is the board outline layer - just check it for each Gerber layer and then process the CAM job. 

This is discussed more in part two of the tutorial I linked.

[Jon Chandler]

Here's a pic showing the above...tabs are actually at the top.

[AlfBaz]

Thanks Jon, I use altium and thanks to your info I had a better look at the cam gen dialog...
Right next to the column that allows you to select what layers to generate is another column that says layers to include in all plots

[poorchava]

I typically do it on silkscreen layer. And in my email with gerbers i make it VERY clear that board outline is in file xxxxxxx.GTO

[AlfBaz]

I don't understand why the outline isn't on a layer on  its own

[mickpah]

hi
go to this link http://imall.iteadstudio.com/open-pcb/small-batches-pcb/im120418021.html , then click on download
the drc and cam jobs for itead are there.
Once I have created the gerbers what i do is is check the gerbers with is tool http://gerbv.gpleda.org/ to ensure that match my design
has worked for me so far.

[mrflibble]

I typically do it on silkscreen layer. And in my email with gerbers i make it VERY clear that board outline is in file xxxxxxx.GTO

Just got my first PCBs from itead, and same here. I put the outline on top silk, and that went just fine. Good plan to explicitely mention it in email though, I'll do that as well for the next batch.

Now that I think about it ... will that email remark get communicated down the line? For all we know it's order # + zip file and lob it to the factory guys. In any event, it probably doesn't hurt to add it to the email.

[Jon Chandler]

I used to include the board outline in the just the top silk layer and it worked fine many times.  But then I had an order that seemed to be stuck.  When I inquired, I was told there was a problem with the Gerbers and they had sent an email about it.  No such email had been received, so I asked them to send it again (why they didn't say what the problem was when I asked, I'll never understand) and the response was that they couldn't find the board outline.

Putting it just on the silk layer had worked fine six or eight times;  as Murphy would have it, when I was in somewhat of a hurry to get the board, it didn't work.  So now I just include it on every layer and there can be no doubt.  It's just a matter of clicking a box on each layer in the CAM file (which has now Ben saved with the changes) so it's no extra effort to include it.

[poorchava]

I had to clarify some stuff once (regarding them suspecting i was trying to panelize with long slot, which I wasn't) and communication with itead was not that bad, especially when compared to your typical chinese supplier. And obviously is may be the dialog between itead and the factory that sucks, not necessarily itead themselves

[ve7xen]

I include the outline on the top silk as well as provide a separate gerber for the board outline. No idea which they use, but it can't hurt. Unless they think it's a copper layer or something

[Dagon]

I usually just stick it in one of the top layers. Never mentioned it in the mail, never had any problems.

On a different note, just noticed they do flexible pcbs now, that's kind of cool.

[gregariz]

I don't understand why the outline isn't on a layer on  its own

I include it in a layer on its own. ie a .gko file

I think including the keepout/board outline in a layer like the lop layer etc is somewhat confusing / non-standard practice. In a file where internal cutouts are needed in the .gko I imagine it could be unworkable to include them in a signal layer.

[AlfBaz]

I think including the keepout/board outline in a layer like the lop layer etc is somewhat confusing / non-standard practice. In a file where internal cutouts are needed in the .gko I imagine it could be unworkable to include them in a signal layer.

My thoughts exactly

[mrflibble]

Trying to figure out what the best practice would be for outlines. So far I've done them in top silk, but I can see how this would be a bad idea.

As for using the .gko as board outline, see for example this bit:

"The keepout layer is intended to be used by the automation in Protel to guide the automated parts placement as well as the auto router by defining areas within the design that should be avoided by these functions.

This function allows the designer to outline the areas available for these functions thus excluding all other areas.  In many designs this boundary is the same as the boards’ outline and for some designers this is always that case so for them the keepout layer (output as the .gko Gerber file)  has become synonymous with the board outline.

However, many designers actually use the keep out layer for its' intended function and thus this does not represent the outline.  These causes a lot of confusion because the outline in the keepout layer is often very similar to the board outline but not exactly the same.  It is because of this that we do not assume that the .gko file should be used to represent the board outline.

Protel offers multiple mechanical layers that are intended for supplying the outline in the CAD data (typically the .gm1 and .gm4 layers are used for this purpose) or the outline can be added to the drill drawing (.gd1 as an example).  We suggest that you use these layers for supplying not only the drawn outline, but also add confirming dimensions to these layers as well.  If your design protocol requires the use of the .gko files for representing the boards outline please detail that the .gko files should be used for the outline in a readme file or in the Fabrication Print.  Otherwise your order will be placed on CAM hold pending this confirmation."

So for future pcb's I think it just might be best to put the board outline on a seperate mechanical layer. Is there any prefered standard, or is Mechanical 1 just as good as Mechanical 3? Right now I have mechanical 3 as the board outline and mechanical 4 as panel outline. For straight up pcb gerbers I can then use mechanical 3 as the outline for gerbers, and when I want to combine boards onto a panel I draw the new outline on mechanical 4. That way I don't have to edit my pcb source files just because I happen to want to put it on a panel this time.

Anyways, is there any standard? Apart from the "so many standards, you can always pick on you like" kind of standard.

And suppose you put your outline in a seperate gerber, what do you call it? .GM3 / GM4 in the above example? Something else?

[gregariz]

In my experience .gko has been the most commonly used file extension for a board outline but the way I see it as long as the board outline is in a separate file you can rename it to whatever you like. I notice that batch pcb simply like to call it something like .outline

Programs like mentor call everything with the same extension. Something like .pho IIRC (for photoplot). There doesn't seem to be much of an agreement with regard to names, other than you see alot of .gko. I've seem some programs just number them. Rimu used .g26 for all outlines.

.gm seems to be a reasonable one to pick, however my understanding was that some of those were for mechancial operations like countersinking and v-scoring, so that may confuse other people.

Sorry.. not much help. Maybe .outline is safest.

Edit: I would add that when I worked with some of the larger companies that have specialized cad people, usually orders are accompanied with a 2D autocad type drawing where instructions and dimensions are given so any confusion about what the final article should look like is addressed.