How to efficiently use the Eagle autorouter function?

[sandeep4386]

Eagle autorouter

Hi folks,
I am designing a PCB for one of my project. I have drawn schematic for it and now I'm routing the board. I have tried eagle autorouter function and it is routing around half of my design however I'm finding,remaining half is really difficult for me to route manually.
May I know, Is there any way so that eagle autorouter will do most of the job for me? :lol: Furthermore, I am attaching schematic and board layout with this post. Please do let me know if you have any suggestions for me regarding efficient component placement and other aspects of design. I have to sumit this design in a day so I'm kinda messed up right now. Any help would be highly appreciated. Thanks.

https://obrazki.elektroda.pl/35_1285204868.png

https://obrazki.elektroda.pl/27_1285204868.png

 

[sanjubluerock3]

Re: Eagle autorouter

as per your board design which u have done is with auto route but i suggest u to use manual route ,main thing is u need to place the components such that it should not jumble and u have not selected ratsnest option....
and by seeing your schematic i think you are using smd components...so the board should be double layer....

this video tutorial link might help u to design a nice board...


YouTube - Eagle Tutorial Lesson 1

and please contact keith1200rs he is very helpful... in designing board

https://www.edaboard.com/members/257767/

 

[keith1200rs]

Re: Eagle autorouter

I don't use the autorouter, but the key to routing a board manually or otherwise is firstly the placement. If you don't place the components well then the routing will be difficult or impossible however you do it. Where you get a bottleneck (such as where you have the long connectors) then you need to consider giving more space for tracks on either side. Sometime rotating a component through 90 or 180 degrees will help. If the connector pins aren't pre-defined then you can often move them around for easier routing.

When setting up the autorouter there are quite a few things to set. The grid is an important one. A smaller routing grid will slow down the routing but make it more likely that it will finish. With conventional 0.1" components a 0.05" grid was often OK but with surface mount components of varying pitch it is often necessary to go down to quite small grids. Routing manually I I often work at 0.125mm but sometime have to go smaller. It makes sense to keep your routing grid associated with your minimum track width and spacing. So, if your minimum track is 10 thou then a 10 thou or 5 thou routing grid makes sense.

Keith.

---------- Post added at 09:00 ---------- Previous post was at 08:58 ----------

By the way, I wouldn't bother to autoroute a board like that. You will get a better layout doing it manually (after you have learnt how to do it well).

Also, you have some drawing errors - apparent connections on the schematic with no junction. Run the error checker in the schematic and sort out the errors before you start routing the board.

Keith.

 

[FvM]

Re: Eagle autorouter

To add a few comments to Keith's valuable points:

- You usually want power supply nets wired with a larger trace width than signal nets. For auto router operation, it's required to set all design rules, including net properties before you start the routing, it's also highly recommended with manual routing.

- The capacitors C1 - C4 are apparently intended as bypass capacitors. To be effective, they should be placed near the components that need supply bypassing.

- I guess, the Eagle autorouter stopped due to an unsuitable routing grid and/or minimum distance setting. It should be able to route most nets of the present design.

But I agree, that manual routing gives neater and mostly better results. A compromise may be to route power supply and critical analog/high speed nets (if any) manually, protect them and let the ordinary signal nets to the autorouter. I'm not sure about the results with Eagle, but it's a promising method to speed up PCB design with industry standard tools like Specctra.

 

[keith1200rs]

Re: Eagle autorouter

One other thing I forgot - you can set the preferred routing direction for each layer. For through-hole components it doesn't matter much, but with surface mount it can make an impact if you pick the wrong preferred direction. In your case I would suggest that the top layer should be routed horizontally.

Keith.

 

[sanjubluerock3]

Re: Eagle autorouter

i hope by now u have an idea how to route it perfectly....from all the suggestions by experienced people...keith and fvm...

 

[sandeep4386]

Re: Eagle autorouter

as per your board design which u have done is with auto route but i suggest u to use manual route ,main thing is u need to place the components such that it should not jumble and u have not selected ratsnest option....
and by seeing your schematic i think you are using smd components...so the board should be double layer....

this video tutorial link might help u to design a nice board...


YouTube - Eagle Tutorial Lesson 1

and please contact keith1200rs he is very helpful... in designing board

https://www.edaboard.com/members/257767/

Hey thanks for your help. I watched all rpcelectronics videos. They were really helpful.

 

[sanjubluerock3]

Re: Eagle autorouter

thats nice ....ok all the best...

 

[sandeep4386]

Re: Eagle autorouter

I don't use the autorouter, but the key to routing a board manually or otherwise is firstly the placement. If you don't place the components well then the routing will be difficult or impossible however you do it. Where you get a bottleneck (such as where you have the long connectors) then you need to consider giving more space for tracks on either side. Sometime rotating a component through 90 or 180 degrees will help. If the connector pins aren't pre-defined then you can often move them around for easier routing.

When setting up the autorouter there are quite a few things to set. The grid is an important one. A smaller routing grid will slow down the routing but make it more likely that it will finish. With conventional 0.1" components a 0.05" grid was often OK but with surface mount components of varying pitch it is often necessary to go down to quite small grids. Routing manually I I often work at 0.125mm but sometime have to go smaller. It makes sense to keep your routing grid associated with your minimum track width and spacing. So, if your minimum track is 10 thou then a 10 thou or 5 thou routing grid makes sense.

Keith.

---------- Post added at 09:00 ---------- Previous post was at 08:58 ----------

By the way, I wouldn't bother to autoroute a board like that. You will get a better layout doing it manually (after you have learnt how to do it well).

Also, you have some drawing errors - apparent connections on the schematic with no junction. Run the error checker in the schematic and sort out the errors before you start routing the board.

Keith.

Hey thanks Keith for your valuable guidance. I tried manual routing and now I am liking it. I have one question for you. I need to drill holes at four corners of PCB for mounting. How can I do this in Eagle?

---------- Post added at 06:18 ---------- Previous post was at 06:17 ----------

To add a few comments to Keith's valuable points:

- You usually want power supply nets wired with a larger trace width than signal nets. For auto router operation, it's required to set all design rules, including net properties before you start the routing, it's also highly recommended with manual routing.

- The capacitors C1 - C4 are apparently intended as bypass capacitors. To be effective, they should be placed near the components that need supply bypassing.

- I guess, the Eagle autorouter stopped due to an unsuitable routing grid and/or minimum distance setting. It should be able to route most nets of the present design.

But I agree, that manual routing gives neater and mostly better results. A compromise may be to route power supply and critical analog/high speed nets (if any) manually, protect them and let the ordinary signal nets to the autorouter. I'm not sure about the results with Eagle, but it's a promising method to speed up PCB design with industry standard tools like Specctra.

Thanks FvM. That was really helpful.

 

[sanjubluerock3]

Re: Eagle autorouter

to drill holes at four corners of PCB for mounting just click on draw tab an select hole or i use circle option and set the dia ...

 

[sandeep4386]

Re: Eagle autorouter

Great. Thanks.

 

[sandeep4386]

Re: Eagle autorouter

Hey guys, I need to connect standard 20 PIN JTAG male header on my PCB. Can anybody tell me whether eagle has this part? If yes, in what library is it?

---------- Post added at 03:05 ---------- Previous post was at 02:44 ----------

Found the library for 20 pin standard jtag male connector. However I am not able to find this part on digikey or mouser. Where can I buy this 20 pin Jtag connector. Please pour ur views.

 

[FvM]

Re: Eagle autorouter

I need to connect standard 20 PIN JTAG male header on my PCB

I doubt that there is one standard 20-pin connector usual for JTAG, I have already seen many. You should better specify the pin grid and possibly connector shape.