How to fix red circle dimension error in Eagle

[Anonymous]

I am new to Eagle. I am not an electrical engineer, but I an trying to learn. I am creating a 6 layer board for my circuit. However I ran into this dimension error where I have red circles around all of the pins. I don't know what to do exactly, because these are the dimensions of the components, so I can't change them. How should I go about fixing this? Thank you for your help. -Cole

[rachaelATWH4]

Hi Cole,

A couple of things:

1) Are these components you have created yourself or are they straight from the library or from somewhere else?

2) Have you set up your DRC correctly, either by loading an appropriate DRC configuration file or by manually setting the parameters to match your board manufacturers capabilities?

If you haven't set up the DRC correctly then this can lead to lots of errors showing like this as the EAGLE default DRC settings are very conservative.

Best Regards,

Rachael

[Anonymous]

Thanks for your help!

I did create the parts myself. I used a solidworks sketch of the pin layout, placed pins over the sketch to make sure they were the right size for the components. So I think they should be the right size, but I don't know if i maybe missed something.

I have left the design rules default. I tried to mess around with them a bit, but I couldn't figure out what I needed to change. I have defined the board to be a 4 layer board however. But that's where I'm stuck. I don't know what to change in the design rules to fix this error.

Thank you!

-Cole

[rachaelATWH4]

---

@Anonymous wrote:

I have left the design rules default. I tried to mess around with them a bit, but I couldn't figure out what I needed to change. I have defined the board to be a 4 layer board however. But that's where I'm stuck. I don't know what to change in the design rules to fix this error.

---

Hi Cole,

Where are you having your PCB manufactured? The PCB manufacturer will at the very least be able to supply a list of all their design rules which you can then enter into EAGLE. However, a lot of manufacturers actually supply EAGLE .dru files for various board stack-ups. Eurocircuits and Wurth and two examples of manufacturers who supply dru files and you will find these are already available in the dru folder in your EAGLE installation directory. To use them open the DRC and choose the "Load" option and navigate to the .dru file you intend to use.

Best Regards,

Rachael

[edwin.robledo]

Hi,

It appears that you may have drawn your component outline shapes on the Dimension layer.  The dimension layer is intended to be used to define areas that are going to be cut off the board.  For then it will flag a Dimension error.  The same will occurs if you place copper close to a hole that has been placed using the HOLE command. 

I hope this helps.

Ed

[Anonymous]

Hey Rachael,

Thank you so much. I had no idea. I will give that a try. I am probably using OSHPark. So I will see if they have any file like what you described.

-Cole

[rachaelATWH4]

---

@Anonymous wrote:
Hey Rachael,

Thank you so much. I had no idea. I will give that a try. I am probably using OSHPark. So I will see if they have any file like what you described.

-Cole

---

Hi Cole,

OSHPark do have EAGLE dru files so you'll be able to get them from their website.

Best Regards,

Rachael

[Anonymous]

I see, so what you are saying is I put the copper pads on the dimension layer when creating my custom parts?

Does that mean is should just go back into my library and redo them making sure I place them on the right layer? What layer should I place them on?

Thank you for your help!

-Cole

[rachaelATWH4]

---

@Anonymous wrote:

I see, so what you are saying is I put the copper pads on the dimension layer when creating my custom parts?

Does that mean is should just go back into my library and redo them making sure I place them on the right layer? What layer should I place them on?

Thank you for your help!

-Cole

---

Hi Cole,

I don't think you could have put your copper pads on the dimension layer unless you drew the pads by hand with a polygon rather than using the PAD tool, but it doesn't look like you did that. I think Ed was referring to the component body outline which you should draw on tPlace (making sure not to overlap pads) and also on tDocu (so you can create a nice assembly drawing). I'm not sure that this would cause all of the errors you are seeing though.

Best Regards,

Rachael

[Anonymous]

Sorry I am really new to this. What part is the component body outline?

-Cole

[jorge_garcia]

Hi @rachaelATWH4,

@Anonymous Mentioned that he used a solidworks sketch to design the part. Being that the case it's likely that he imported the DXF to the dimension layer so all of the holes for those pads have a feature on the dimension layer and that's what Ed thinks is causing the issue.

Like you mentioned if he just switches those circles and outlines from dimension to tDocu to tPlace then those errors should hopefully go away.

Let me know if there's anything else I can do.

Best Regards,

[Anonymous]

That's exactly right, I am using DXF files. So are you saying that the DXF that I am importing needs to be on a different layer?

-Cole

[rachaelATWH4]

---

@jorge.garcia wrote:

@Anonymous Mentioned that he used a solidworks sketch to design the part. Being that the case it's likely that he imported the DXF to the dimension layer so all of the holes for those pads have a feature on the dimension layer and that's what Ed thinks is causing the issue.

Best Regards,

---

Ahhhh, I had missed that nugget of information, in which case Ed is 100% right!

Cole,

Given Jorge and Ed's comments, I'm assuming there are circles on this layer marking where all the pins are required to go which should be moved to the tDocu layer only (if needed on the assembly drawing) and not be on tPlace. Only the body outline and silk screen text (i.e. >NAME) should be on tPlace.

FYI, the body outline marks the outline of the body of the part on the silkscreen layer of the board so you can see more easily where things need to be placed when assembling parts onto the board.

Best Regards,

Rachael

[rachaelATWH4]

---

@Anonymous wrote:

That's exactly right, I am using DXF files. So are you saying that the DXF that I am importing needs to be on a different layer?

-Cole

---

Yes, import it into tDocu and then copy the main body outline to tPlace. You have it imported now though so just change the layers on these circles and lines and all should be fine.

Best Regards,

Rachael

[Anonymous]

Awesome! Thank you! I will give that a try.

[Anonymous]

Hi Rachael, 

have you ever tried seeed studio pcb https://www.seeedstudio.com/fusion_pcb.html? their price seems more affordable. 

[rachaelATWH4]

---

@Anonymous wrote:

Hi Rachael, 

have you ever tried seeed studio pcb https://www.seeedstudio.com/fusion_pcb.html? their price seems more affordable. 

---

Hello,

No I haven't used Seeed Studio yet, but strangely enough I was actually looking at their website yesterday. I might give them a try on a small prototype build to see what the quality of their boards is like.

Best Regards,

Rachael