Silkscreen, auto-routing and single layer - DXP 2004

[aredhel]

+dxp2004 +1 layer +route

Hello there I started to learn PCB making using DXP 2004 and use **broken link removed** site for a short tutorial. I have a few questions on DXP 2004:

1. How do I view my silkscreen? Somehow I could not find it. Even the "Help" files are giving me problems.

2. Auto-routing: all I have to do is place the components inside the PCB board and then "Auto Route >> All" ... right? All of my components have their own ready-made footprints, so there are no custom footprints in my design.

3. Is it possible to create my PCB using DXP 2004 with only 1 layer, because the auto-routing connection shows red and blue lines. So that is a 2-layered PCB, top and bottom and that kind of PCB board is rather expensive ... around 40 where I come from and I want to cut cost.

Hope someone could help me.

 

[s_cihan_tek]

create a pcb from a schematic dxp2004

I'm using Altium Designer, not DXP. But probably answers to your questions will be same for both packages.

1- Press "L" to open the view configurations window and disable all layers except silkscreen layers. I don't know any other way to see the silkscreen layers alone.

2- You just need to open the Design Rules window and from there under the Routing/Routing Layers section, remove the tick from the "Allow Routing" column for the other layer.

3- If you do the thing above, you would be able to continue as if its a 1 layer project.

Regards...

 

[Anonymous_Ricky]

auto route dxp2004

hi,
Silkscreen layer in DXP is named as Top nad bottom overlay so if you want to see silk legend of a PCB you have to turn that layer on.
rest of your question have the same answer from me as above.
Regards

 

[aredhel]

+dxp2004 +1 layer

Thank you guys. By the way when I click on "PCB Board Wizard" it asks for the "signal layers" and "power planes". Since I want mine to be on one layer, does that mean:

Signal layers = 1
Power planes = 0

It seems like the default signal layers is 2 because I can't seem to change it.

--------

From the attached PCB picture, I used auto-routing and I am wondering why are there double line/track at the bottom left connection to capacitor C7? It is not just C7, but others as well. Anyway thank you again to those who replied !

 

[s_cihan_tek]

dxp 2004 1 layer

Thank you guys. By the way when I click on "PCB Board Wizard" it asks for the "signal layers" and "power planes". Since I want mine to be on one layer, does that mean:

Signal layers = 1
Power planes = 0

It seems like the default signal layers is 2 because I can't seem to change it.

Altium doesn't allow creation of a pcbdoc which has less than 2 signal layers. Therefore if you want to make a single layer PCB, you shold set the signal layer count to 2, plane count to 0 and forget about the second signal layer in the created PCB because you won't be using it.

From the attached PCB picture, I used auto-routing and I am wondering why are there double line/track at the bottom left connection to capacitor C7? It is not just C7, but others as well. Anyway thank you again to those who replied !

I don't know the reason but most autorouters i've used until now make that kind of weird things. Just delete them.

 

[me_guitarist]

dxp bottom overlay

Hi guys,

May I know where can I download component library for DXP2004?

 

[House_Cat]

dxp single layer auto route

The performance of the autorouter depends heavily on the Design Rules you set before starting the router. Allowed clearances and the short circuit rule are particularly important. I see some shorts on your board, indicating that the rules weren't set up before the router was run.

To remove the double tracks, you can use "Design>>Netlist>>Clean All Nets".

When routing a single layer board, you would set the Design Rule for Routing Layers by unchecking all of the layers except the one you want the autorouter to use. You are really making a two layer board (Top and Bottom). You've just chosen to only use one side.

There is no autorouter in the world that will do a 100% clean route of all paths. Once you've allowed the software to do the routing, you'll have to manually clean up.

Looking at the picture of your board, I would offer the following advice. Group your components as they are grouped in the schematic. The way you have laid out the board isn't conducive to a clean route. For example, the filter network connected to pin 3 of U5 should be grouped as it is in the schematic instead of spread out on either side of the IC. If you keep the grouping in the order of the signal flow, you'll have the shortest tracks on the PCB. The autorouter results will be cleaner, and your signals on the finished board will also be cleaner.

I don't see net names on some of the schematic wires. Unnamed wires will be assigned system net names, and if not connected on both ends can get connected together or just not connected by the autorouter. Did you look at the "Messages Panel" when you compiled your schematic? Errors and warnings are listed there after the compiler does the electrical checks.

------------------------------
Altium no longer offers a download for DXP2004 libraries, but they have the libraries for DXP2002 at https://www.altium.com/altium/altiu...braries/en/dxp2002-release-libraries_home.cfm

 

[aredhel]

single layer dxp

The performance of the autorouter depends heavily on the Design Rules you set before starting the router. Allowed clearances and the short circuit rule are particularly important. I see some shorts on your board, indicating that the rules weren't set up before the router was run.

Here is a new PCB design and I have done the "Clear All Nets". As for "Clearances" and "Short Circuit" design rules, I have not set them up because I am not sure what I should tweak. As for Pin 4 of U6, you can see the track almost touches the pin and then it makes some sort of a U-turn. So I should adjust this then?

The only design rule that I set for this is the "Routing Layer" where "Bottom layer > Vertical".

I don't see net names on some of the schematic wires. Unnamed wires will be assigned system net names, and if not connected on both ends can get connected together or just not connected by the auto-router. Did you look at the "Messages Panel" when you compiled your schematic? Errors and warnings are listed there after the compiler does the electrical checks.

As for the net names, you mean the names are supposed on the schematic to appear in the PCB? If that is the case then I am not really sure how I should do that. I did compile my schematic where I did "Project > Compile Schematic XXX", however no "Messages Panel" appears. When I created a new PCB and did "Design > Update PCB XXX" ... no errors appeared. Also when auto-routing was done, there were no failed connections and contentions.

 

[House_Cat]

dxp 2004 change layer name

Both your schematic and your PCB look better than the first attempt - particularly the schematic. The design rules are pretty self explanitory. For the type of board you are now doing, you should look at the rules under the "Electrical" and "Routing" headings in the Design Rules dialog. The rest of the rules deal with more advanced boards that need special handling because of manufacturing or signal integrity issues.

What I meant about your net names was that your schematic didn't have all nets named. Your new schematic appears to be fine. Whenever you have a wire that is connected only on one end, you should assign the wire a net name to tell the software where it should be connected.

Your PCB still needs cleanup. The first thing to do is to look where there are opportunities to simply rotate the components to shorten traces. For example, if you rotate C11 180deg, the tracks are shorter and simpler, likewise with JP2 and some of the other components.

Your gnd circuit is going to cause you problems because of the way it is strung out all over the board. Since you are using thru-hole components, I would consider using a polygon plane on the bottom layer for GND. The board would be a bit more complicated to make at home (both sides of the board would have to be etched), but it would be more professional when completed.

If you would like for me to do some cleanup to illustrate what I mean, you can zip or rar a copy of your files and PM them to me. I'll do a bit of cleanup, and send them back so you can see what sort of things can be done.

 

[aredhel]

dxp assigning nets to a layer

OK here is the track with a bypass capacitor (with and without ground polygon on one layer) and I have done a bit of cleaning, but I am not sure if it is still messed up. Anyway if I want to do double layer which side should I put the components: the ground plane or the track? My soldering skills aren't that good.

 

[KP]

dxp 2004 one layer rule

Latest Winter09' Design Rules -
'Silkscreen over Component pads' is controlled by Machine Not Human anymore
Do it Just Right at a first time...
Thanks to Altium

See video clip attached.

 

[aredhel]

dxp silkscreen over component pads

OK thanks for the help guys!