Continue to Site

Welcome to our site!

Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.

  • Welcome to our site! Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.

custom pcb maker who can take seetrax ranger file format .rxl

Status
Not open for further replies.

natek83

New Member
I need to find a pcb fab that can use the seetrax ranger software. The demo version is free and is fully functional for this layout because it has less than 30 parts or something. I was given the pcb layout by someone else and don't have any experience doing pcb layouts. I attached the file if anyone wants to have a look. Can anyone give me a recommendation of where I can get this made? Thanks
 

Attachments

  • sei..zip
    13 KB · Views: 132
Have you actually laid out the PCB? All PCB manufacturers work on Gerber files and Seetrax enables you to generate Gerber files once you have laid out the PCB. You want to try to make your PCB single sided to reduce the cost of the PCB. I suggest you look in the help files of Seetrax (I think they are buried in one of the program directories) and work your way through a sample design. I started using Seetrax about 5 years ago and although it is basic, it is a very neat program to use and does everything I have ever needed
 
Thanks a lot for your help. I found a section in the getting started guide which mentions creating a gerber file but its extremely vague.

I'm supposed to pick one of these options but I'm not sure which:

New Schematic Output - use to output all schematic
sheets
New Solder Paste Output - use to output automatically
generated solder pastes – these will have
uniform pad decrease in size
New Solder Mask Output - use to output automatically
generated solder masks – these will have
uniform pad increase in size
New Drill Sheet Output - use to output an automatically
generated drill drawing
New Artwork Layers Output use to output all other
artwork data, including copper, silk-screen,
documentation, power plane and user-defined
solder mask & solder paste layers
 
Last edited:
Well I realized the correct option was "New Schematic Output" and was able output a gerber file. trying to check if I did it right atm.
 
Nevermind, "New Schematic Output" isn't what I need to do. Which of the options would it be? Solder mask/solder paste/drill sheet/artwork?
 
Ok well I tried artwork and I added some layers to the output and the gerber file now shows what looks kind of like traces but they're kinda funky compared to the "artwork" inside the .rxl. I believe I need 3 different gerber files since its a single layer with no drilling. These would be:

"Artwork, top side: Layer V and T Pads, plus Layer T copper

Top silk-screen: Layer 1 and 2 copper

Top solder mask: Layer T pads
If vias should be exposed through the solder mask, then also Include vias
from the Setup window and include layer V pads."

What are vias exactly?

Then I think I save each gerber file with a specific file extension for their job.

Top copper .GTL
Top solder mask .GTS
Topsilkscreen .GTO

Is that at all close to what I need?
 
Last edited:
Here goes. PCBs are made up of a series of layers. For a single sided PCB, you will have your copper on the bottom together with a solder mask. the solder mask is the green laminate that they put over PCB tracks to stop the solder flowing all over the PCB tracks. Obviously you want to keep the PCB pads exposed so they can be soldered to.

Also for a single sided PCB, you will have a silkscreen on the top layer that shows the outlines of all your components. This is just another layer of the PCB and you have to tell the PCB maker that you want this as silkscreen and not copper (see below). Seetrax recommend that you have your component outlines on layer 3 and your text on layer 4. You then go on to specify (see below) that you want these layers as silkscreen.

With a 2 sided PCB, you will also have a top layer of copper (track on the top of the PCB). This can be added as an extra layer. If this is the case, once you have designed your PCB, you need to specify that you want your top tracks as copper.

Vias are plated holes that are drilled through the PCB. They link the top layer of the PCB with the bottom layer. If you have a single sided PCB then you will not need vias.

Below are some notes I made for myself years ago when making PCBs. It is also probably best if you phone Seetrax and ask them to send you a pdf of the instructions. I have a copy on my PC, but am not sure about copyright etc. They are very helpful

The notes below apply once you have laid out your PCB




Creating Outputs:
Set data format to Excellon
Set Units to Inches
Save Drill Data
Save Rout Data
Save Tool Data

Saving Gerbers in Olimex format:

Select Photoplotter -> Setup -> auto job dcode table – Go into Properties and Selected dCodes as extended Gerber

Select Solder Mask -> Setup
In Setup
Set pad swell to 0.015”
Set X shift to 1.000
Set Y shift to 1.000
Tick Plot Profile box to define edge of board
Tick Plot Target box
Tick ‘Include Vias’ Box if you have used Vias or wire links
In Layers Selection
For Bottom Solder Mask:
Select what you DO NOT want covering
Tick Bottom + Pads only (to stop them being masked)
Tick V + Pads if vias and wire links are included


Close dialogue box
Do Plot Preview (next to GO button)
Hit the GO Button
Save file as Bottom Solder Mask.ger

For Top Solder Mask – only if you have tracks on the top layer. If you have vias and you print a top layer, you will get solder pads on the top layer:
Select what you DO NOT want covering
Tick Top + Pads only (to stop them being masked)
Tick V + Pads if vias and wire links are included

Close dialogue box
Do Plot Preview (next to GO button)
Hit the GO Button
Save file as Top Solder Mask.ger


Select Artwork Layers -> Setup
Select Plot Targets box
Select Plot Profile box
DO NOT select Plot Keepouts or your keepouts will come out as copper
In Layers, select Bottom Layer: Pads and Copper
Select V layer Pads if you have wire links or vias
Do Plot Preview
Hit the GO Button
Save file as Bottom Copper.ger

If you have tracks on the top layer:
In Layers, select Top Layer: Pads and Copper
Select V layer Pads if you have wire links or vias
Do Plot Preview
Hit the GO Button
Save file as Top Copper.ger


Select Artwork Layers -> Setup
In Layers, select Layers 3 & 4: Pads and Copper
Include Layer ‘T’ Copper if you have wire links – this will treat all artwork on the top layer as Silkscreen, not copper
Do Plot Preview
Hit the GO Button
Save file as Top Silkscreen.ger
 
Status
Not open for further replies.

Latest threads

New Articles From Microcontroller Tips

Back
Top