Partial autoroute

Info wrote on Wed, 04 August 2010 17:16

Is it possible to auto route just a partial part of the board?

Yes.

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

I do not think you can say route lower left of schematics (or any rectangle)

But you can do auto on signals like gnd vcc like this

AUTO  GND  VCC

Christen Fihl

Harry H. Arends wrote:

Is it possible to auto route just a partial part of the board?

Searching in help for restrict gives:

"If required, restricted areas for the Autorouter can be defined as

RECTangles, POLYGONs, or CIRCLEs on the tRestrict, bRestrict, or

vRestrict layers. Note: areas enclosed by wires drawn on the Dimension

layer are borders for the Autorouter, too. "

On 8/4/2010 5:16 PM, Harry H. Arends wrote:

Is it possible to auto route just a partial part of the board?

Hi Harry,

If your not as command line inclined, you can click on the autorouter

icon. When the dialog pops up look at the bottom of the screen you'll

see a select button click it.

Now EAGLE will allow you to select the signals you want to route. Once

your done selecting click the GO button and the autorouter will route

the selected traces.

hth,

Jorge Garcia

Cadsoft Computer

Harry

Seems like we cannot tell exactly what you mean.

- Olin just had his standard autoanswer on, correct in both cases anyway

- Jorge and myself read question as some signals and not others

- Morgan might have read question correctly by pointing you into restricting

board usage

Maybe you could pinpoint which of the two interpretations you had in mind,

maybe a third one

Christen

Am 04.08.2010 23:16, schrieb Harry H. Arends:

Is it possible to auto route just a partial part of the board?

Just a random guess but maybe through laying a STOP polygon around the

areas you dont want to route and later removing them.

On 5/30/2011 10:52 AM, Dominic Hoeglinger wrote:

Am 04.08.2010 23:16, schrieb Harry H. Arends:

>> Is it possible to auto route just a partial part of the board?

 

Just a random guess but maybe through laying a STOP polygon around the

areas you dont want to route and later removing them.

a polygon in the stop layer makes holes in the solder mask. the restrict

and keepOut layers can be used to control where traces are routed and

components are placed. but I think the question is whether individual

nets can be autorouted or left unautorouted and the answer is yes. HELP

AUTO for info.

Gary Gofstein wrote:

On 5/30/2011 10:52 AM, Dominic Hoeglinger wrote:

>> Am 04.08.2010 23:16, schrieb Harry H. Arends:

>>> Is it possible to auto route just a partial part of the board?

>>

Autorouting takes place inside the bounds of the board outline in the

dimension layer20.

If you wish to autoroute a small area, the following works:

1) Move your board outline to another user defined layer (temporarily)

2) Draw an outline around the area to be autorouted (in layer 20 Dimension)

3) Autoroute

4) Restore the board outline to the correct layer

Airwires not ending within the boundaries do not get routed.

HTH

Warren

My previous post was written poorly and does not really work as described.

After a bit more testing on more complex designs:

Autorouting happens within the extremities of your design (components) and

limited by a dimension line outside of that area. If you draw the board

outline in the middle of your design the autorouter will route airwires

inside and outside that outline but not those that cross the outline.

Now, to recover from my previous post, it can be made to work the following

way:

Block out 'all' the area of your design that you do not want routed using

rectangles, or draw a polygon, on the 20-Dimension layer leaving only the

area of interest. You can leave your board outline, no need to move it to

another layer.

The exposed area alone will route. Airwires beneath the rectangles/polygon

and emerging from it will not route.

Remeber that there is a DRC setting for copper clearance from items in the

dimension layer so when you build the area to route make it a little

larger.

Deleting this 'blocking' from the Dimension layer later maybe safer/easier

than using the Restrict layers. This technique masks both the top and

bottom layers at the same time making it quicker than the restrict method

when identical top/bottom masking is required.

Try it, it's very workable.

I've attached the experiment I did with Hexapod from the Examples folder.

The first images show an airwire in the top right that looks like it should

have been routed and is not. I suspect this is to do with the DRC distance

settting keeping traces away from dimension layer objects. When I opened up

the polygon a little more as in the last image the routing occurred.

Warren

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.