3
\$\begingroup\$

As you can probably tell, I'm new to PCB design and recently did a design of a DIY circuit. Everything looks acceptable (to me), however for some reason I cannot align the PCB edges to the polygon edges (see picture below). Is this going to affect the production? How can I align them properly? (I tried to do it manually but it doesn't work, they won't align).

enter image description here

Technically speaking I don't care if the PCB gets made shorter due to this detail, since it won't affect tracks or components placing (but I'd like to understand what is going on). Also, the ERC check seems to be fine, while the DRC is giving me some warnings I have troubles in understanding:

enter image description here

The vector font warnings are related to the text on dimension arrows (which will not get printed anyway) while all the remaining 34 width warnings are somehow related to the tip of the dimension arrows. Could someone please explain me what is going on? Thanks!

I'm using Autodesk Eagle.

\$\endgroup\$
  • 1
    \$\begingroup\$ When you want things aligned out of the grid (so you cant do it by clicking), you can open the properties and input the coordinates manually. But as Dave said, that shouldn't be a problem for pours, cause they'll be constrained by the dimensions and the margins (copper to edge). \$\endgroup\$ – Wesley Lee Jan 27 '18 at 13:11
  • 1
    \$\begingroup\$ Do not put dimensions on the copper layers. Place them on the "Measures" layer. This will ensure you don't get any errors related to them. If you put dimensions on a copper layer inside the boards, they would end up being in the final Gerber output. \$\endgroup\$ – Tom Carpenter Jan 27 '18 at 14:56
3
\$\begingroup\$

As pointed out already, you do not need to worry about lining up the polygon with the board outline. Polygon pours will be automatically clipped to the outline assuming that the Orphans setting is disabled.

If Orphans on the polygon is enabled, you simply have to get the polygon close enough to the board outline that the board edge to copper clearance setting in the DRC is large enough to remove any trace of the polygon


In terms of your errors (these are errors, not warnings!), they are coming from the fact you are using the wrong layers for things.

The DRC indicates the errors are coming from Layer 1, which indicates that you have put your measurements (dimension arrows (*)) on the Top copper layer (1). You should never do this.

If you put measurements on a copper layer, especially inside the board outline, the measurements will appear in the final Gerber output as copper. This is why the DRC generates errors.

All measurements should be placed on the "Measures" layer (47). This is a layer which is ignored by the DRC and will ensure you don't get any errors related to them. It is safe to use this layer for this purpose as it won't typically produce any physical output


Note (*): There is some confusion between the name "Dimension" which is the name of the tool to draw measurements, and the Dimension layer (20). These are actually two completely different things.

The Dimension layer is where you draw your board outline. The "Dimension" tool is used to draw measurements.

This is basically a really bad naming choice for the dimension tool when it was first introduced. Ho hum.

\$\endgroup\$
  • \$\begingroup\$ This is a very comprehensive answer. Thank you very much! \$\endgroup\$ – mickkk Jan 27 '18 at 20:50
3
\$\begingroup\$

It really doesn't matter if the drawn polygon "slops outside" the PCB dimensions — the actual "pour" that gets generated will be constrained by the design rules to some setback inside the edges of the board. You'll see the actual generated shape if you run the ratsnest command.

Regarding your other errors, you really shouldn't have the layer with the drawn dimensions, arrows, etc. in it selected when you run DRC. Select only the layers that will actually be used for the fabrication. Also, you should not be putting that kind of documentation in a copper layer (Layer 1) in the first place.

In fact, I tend to run DRC on individual layers, one at a time, to get rid of most of the initial problems, before running it on the whole set to catch the inter-layer issues.

\$\endgroup\$
  • \$\begingroup\$ There is no problem in keeping the dimension layer active during DRC checks. The problem here is that he's got other things in the dimension layer that don't belong there. These are apparently things that one of the Docu layers should be used for. Running DRC on one layer at a time can be a useful trick, but you also need to run it with at least Dimension, copper, restrict and keepout layers on so that it can catch errors between layers. \$\endgroup\$ – Olin Lathrop Jan 27 '18 at 14:45
  • 1
    \$\begingroup\$ In fact you should have the Dimension layer visible during DRC. That layer (layer 20) is for drawing the board outline on it. In fact it is the Measures layer that the various measurements should be placed on, a layer which the DRC ignores. \$\endgroup\$ – Tom Carpenter Jan 27 '18 at 14:58
  • \$\begingroup\$ @TomCarpenter: yes, you're completely correct. I fixed my wording above to indicate what I really meant. \$\endgroup\$ – Dave Tweed Jan 27 '18 at 23:47
1
\$\begingroup\$

The outline in the dimension layer defines the size and shape of the board. Polygons in other layers have nothing to do with that. If you want the board a little bigger in one dimension, move the corresponding line in the dimension layer.

You should not have anything else in the dimension layer. If you want to add writing to the assembly drawing, do that in the Docu, tDocu, or bDocu layers.

Note that copper polygons won't usually go to the edge of the board. Usually you specify some minimum distance in the DRC settings. This is to mirror the limitations of fabricating the board and the relative position tolerances of the various layers.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.