Force autorouter to connect on bottom WITHOUT forcing entire net to bottom

[Jason_Okstate]

Hi all,

I'm using Ultiboard 10 and have run into a snag. I'll be milling this board on double sided copper board without plated through-holes. I would like all of my traces to connect to my header pins on the back side of the board for ease of soldering. Is there a way to force autorouter to connect to a component on a certain layer WITHOUT constraining the entire net to that layer? I've see similar posts without any real answers other than autoroute and switch to manual when you need to.

Thanks,
Jason

[lacy]

I had an idea, but since you are not using plated through holes it wouldn't have worked. I really don't see a way to do this without using vias or forcing the entire net to one side of the board. This may be possible, but I just can't find it.

Sorry, I know this is absolutely no help to you.

Message Edited by lacy on 11-15-2007 08:08 PM

[Jason_Okstate]

Well, I had a novel idea that gives me a partial solution. Maybe someone can go a little further with it.
I drew keep-out regions around each header and configured them such that copper top was not allowed with in the region. The problem with this though is that Ultiboard gives me a warning about the actual component being placed in the region. Any ideas how to eliminate these warnings?

[lacy]

I haven't used keep in/keep out areas so what I am going to say is just a theory and could possibly not be the correct approach. First I have to ask a question. Does the board route even though you get these warnings? Are these warnings only shown in the spreadsheet? If the answer to both of these questions is yes then you may be able to ignore them.

The only thing that bothers me about my idea is that if you decide later on to send your boards out to have them manufactured then I do not know if it would be acceptable having components in a keep out area (hence the warning that it is giving you about this). If you are doing your own boards then this shouldn't be a problem.

I will let the NI Team address this further as I have reached the limit of my knowledge on this subject.

I hope that I was of some help even though it seems that I haven't come up with any real solutions. 

[kittmaster]

scrap all that mess......here is the easy way to do it

turn off all object filters

Activate only through hole pad filter

select all pads for IC that need bottom only routing

hover over a selected any highlighted pad and RIGHT CLICK and select properties

Go to autorouting tab and UNSELECT top and click ok to accept

Enable routing layers top and bottom in global spreadsheet view

Autoroute board > it will only connect to the bottom side pad now

enjoy

[lacy]

Thanks Chris for your insight into this. This is similar to my technique I was thinking about, but I was going to manually place vias and then run nets to them. This is a better method as the vias are place automatically. There is only one problem that I see. This is the fact that he is not using plated through holes and I believe vias would be considered plated through hole wouldn't they?  Other than this technique I wouldn't know how to accomplish it without the though holes other than forcing nets to the bottom of the board.

Let me know if I a correct in my thinking here, cause I could be wrong.

Message Edited by lacy on 11-18-2007 10:45 AM

[kittmaster]

This goes without saying any time a pcb without plating unless it is single sided by design, will require "via pins" which are sold through companies like t-tech. Or just a plain old piece of solid 24-28 gauge wire soldered on the top and bottom side of the board to complete the connection.

But yes your right, this is the only draw back.

This decision must be made up front so that their aren't two versions of the pcb from prototype to production.

Its a real pita but it sure beats paying 300-500 bucks for production tooling/waiting and hoping for the best......unless your a master designer.....;)

[lacy]

Thanks Chris, I am not sure how he is going to do this other than the methods we have described. I hope he can take our suggestions and come up with a workable plan. Until then, I think I have exhausted all my ideas on this subject. I wish him good luck in creating his board the way he wants.