Through hole parts connected to the top layer

On 18/09/12 21:56, Tor-Arne Forsmo wrote:

Hi. I'm trying to make a board and then send it off to a board house

for etching. I made the autorouter make the traces for me, both top

and bottom traces with vias and all. The thing is that I have both

SMT parts and through-hole parts on my board, but the autorouter

doesn't seem to care. It sends top layer traces to my through-hole

parts, how do I fix this?

 

Route it by hand?

Why do you consider it needs fixing? If you're having a double sided

board made professionally, surely it's going to be through-plated.

Tracks connecting to through-hole components on the top side is not

wrong - it's perfectly normal.

Rob

Yeah I thought about that, but there are alot of through hole components that simply cannot be soldered to on both sides (not by me atleast). Resistors, ceramic disc caps are probably easy to solder on both sides, but how do one go about doing that for a 4700uF 50V electrolytic cap? On my board I have two minijack connectors and a dual sided pot with a switch. The top contact points for these will be completely covered, so this can't be soldered to the top layer. Couldn't this be an issue for professional people aswell? Why do eagle assume that all through-hole components can be soldered to both layers?

I also wonder about those vias. Will a PCB manufacturer care about how many they are? Or can I litter the board with vias and still get the same price? I'm just picturing that they take longer to make

Am 19.09.2012 08:17, schrieb Tor-Arne Forsmo:

Yeah I thought about that, but there are alot of through hole components that simply cannot be soldered to on both sides (not by me atleast). Resistors, ceramic disc caps are probably easy to solder on both sides, but how do one go about doing that for a 4700uF 50V electrolytic cap? On my board I have two minijack connectors and a dual sided pot with a switch. The top contact points for these will be completely covered, so this can't be soldered to the top layer. Couldn't this be an issue for professional people aswell? Why do eagle assume that all through-hole components can be soldered to both layers?

 

Eagle assumes nothing. You assume something wrong. A via is a little

metal pipe connecting bottom and top tracks without any solder. The wire

of a through hole component is going thorough the "pipe" and is soldered

at the bottom only. It does not matter if the top is covered by the

component since the connection to the top is made by the via itself

already. Check the internet for pcb and via.

I also wonder about those vias. Will a PCB manufacturer care about how many they are? Or can I litter the board with vias and still get the same price? I'm just picturing that they take longer to make

 

You get the answer from the manufacturer of your choice...

--

Mit freundlichen Grüßen / With best regards

Joern Paschedag

Tor-Arne Forsmo wrote on Wed, 19 September 2012 02:17

Yeah I thought about that, but there are alot of through hole

components that simply cannot be soldered to on both sides (not by me

atleast).

They don't need to be.  As Rob mentioned, you will get plated thru holes.

Each hole already connects the top and bottom layers even without a wire

thru it and soldered.

Quote:

Why do eagle assume that all through-hole components can be soldered to

both layers?

Eagle doesn't assume anything.  This is dependent on how you set up the

auto router.  However, the defaults are set up assuming plated thru holes

because that's how multi-layer boards are made.

Quote:

I also wonder about those vias. Will a PCB manufacturer care about how

many they are?

Some do, some don't.  This comes down to the pricing strategy of the

particular board house you choose.  Some board houses charge extra for more

than some number of vias per square inch average.  Usually low volume

prototype services don't charge extra for such things because there is

significant margin built into the price already.  The same board house may

apply a complicated formula to give you a quote for high volumes.  They

often don't even tell you what their formula is, They simply give you a

quote for some number of that particular board.

For a two layer board with lots of thru hole parts, there is some advantage

to routing most of the interconnects on the bottom layer.  This allows for

easier editing to make cuts and jumpers and add parts as you find problems.

This can be done with the auto router by setting the layer costs and other

parameters appropriately.  If your interconnect scheme is not too

complicated, you can try to reserve the top layer to be mostly a ground

plane with only the minimum necessary "jumpers" in that layer that can't be

routed in the single plane of the bottom layer.

However, the bigger issue is why are you designing a real board for thru

hole components?  Thru hole makes no sense other than when a part has to

take some mechanical abuse, like a connector.  Otherwise, surface mount

parts are smaller, cheaper, more available, have a much wider selection,

and are easier to solder.

--

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

Eagle doesn't assume anything.  This is dependent on how you set up the

auto router.  However, the defaults are set up assuming plated thru holes

because that's how multi-layer boards are made.

So a board house makes holes for through-hole components like vias, with a conductive connection between the top and bottom layer? I guess I could talk to a pcb house to get the verified.

However, the bigger issue is why are you designing a real board for thru

hole components?  Thru hole makes no sense other than when a part has to

take some mechanical abuse, like a connector.  Otherwise, surface mount

parts are smaller, cheaper, more available, have a much wider selection,

and are easier to solder.

The through hole componets are two minijacks, a pot, two electrolytic caps, a led and a wafer connector. I guess the minijack and the wafer connector could be SMD, but I had little luck finding SMD minijacks and I have loads of through hole wafer connectors laying around. The pot is mounted to the side of the case and it's going to support the weight of the PCB so this has to be a through hole part. The led is mounted behind the minijack and it's pins are going to be bent over it and through the side of the case so I believe it's safer to have the LED as a through hole part aswell. I haven't been looking for a 100uF SMD cap, if they exist then I could replace the through-hole caps for SMD ones.

I'm not sure if you got your answer.  I also had this question and this

is what I did.

From what I understand....

Question: How do I prevent Eagle auto router to use through hole

componenets as vias or join a top layer track to a through hole

components pin.

Answer:  Open and edit the library that holds your component you are

using.  Edit the package (footprint) of the component that you are

using.  You will have to do this for each component footprint that you

are using.  When you are looking at the component and ready to edit,

select the Rectangle button to draw rectangles and now select the layer

you want to use.  In this case you want the tkeepout or bkeepout or

trestrict or brestrict.  Each one can be used to mark an area that must

not have any tracks.  tkeepout is for top layer, bkeepout is for bottom

layer.  In your case, select the t, for top.  Now draw a rectangle over

the pads, making sure its slightly bigger than the pad itself.  Save the

library when done, refresh and voila.  Autorouter won't go near the top

layer of the pin.

http://dangerousprototypes.com/2012/08/08/how-to-eagle-keepout-and-restrict-layers/

--

To view any images and attachments in this post, visit:

http://www.element14.com/community/message/89761#89761

Through-hole parts can be connected to traces on the component layer if plated through holes are used. However if this is done, some parts are difficult to remove without damaging the board. Heavy components like transformers might break from the board if only connected to traces on the component side. Components that need a lot of heat during the soldering process might not properly soldered if  traces at the component side remove part of the heat and only a small surface is available to apply the heat. Connectors, switches and  potmeters might damage the board as a result of mechanical forces applied to that component. It would be nice if the auto router had the possibility to connect selected parts only at the solder side. It would also be nice if connectors, switches and  potmeters could be connected to wider traces. Very often the traces to these components break as a result of mechanical forces. For instance the earphone connector of a portable MP3 player. A wide trace can easily be repaired by soldering a piece of wire over the crack. This cannot be done by selecting the board rules to use wider traces. The auto router should use wide traces  only close to those components and only where board space is available. This way the boards are more reliable and easier to repair.