1
\$\begingroup\$

I am currently trying to route a micro strip for a GPS and GSM antenna on Altium which got some constraints on spacing with ground poured plane like the one shown just below:

enter image description here

This is currently my design below and I need to adapt it to try to match something in similar shape than what is just show above in my text.

enter image description here

I have calculated the parameter of W, T, S using polar software to respect impedance enter image description here Now I need to draw accordingly. I suppose I have to establish a rule but I don't know how to create it specifically only for this microstrip and not for the entire board.

Any help about how to acheive this will be very appreciated.

\$\endgroup\$
3
  • \$\begingroup\$ Your text talks about microstrip, but your Polar screenshot shows a calculation for coplanar waveguide. Be sure you understand the difference and make a deliberate choice about which one you want to use. \$\endgroup\$
    – The Photon
    Jun 22, 2016 at 16:37
  • \$\begingroup\$ I may have not very well expressed myself. The current consideration is a line leading from a GSM module to a micro coaxial connector for pluging the antenna of the GSM module \$\endgroup\$
    – chris
    Jun 24, 2016 at 3:26
  • \$\begingroup\$ You can choose whether to use coplanar waveguide or microstrip, mainly based on which one ends up having a more convenient geometry. \$\endgroup\$
    – The Photon
    Jun 24, 2016 at 3:54

2 Answers 2

Reset to default
4
\$\begingroup\$

Your best bet would be to create a new clearance rule (Design -> Rules -> right-click "Clearance" in the left pane, select "New Rule", open up the new rule you just created (it'll be titled "Clearance_X" where 'X' is the highest number you see) and in the section labeled "Where The First Object Matches", open the dropdown and select "Net". A new dropdown will appear, and you just need to select your RF Antenna net from the list. Then set the clearance in the "Constraints" section. This will apply this clearance rule to your RF antenna net only, and this will ensure that the polygon, components, and other traces are pulled back from this track. Keep in mind you will probably need to repour your polygon after setting the rule (Go to Tools -> Polygon Pours -> Repour All, or shortcut T-G-A).

\$\endgroup\$
2
  • \$\begingroup\$ Just a question about this. What about the components who are on the path of the strip ? I found out that the clearance is well respected from the strip to the ground plane created around the area but where there are some components standing the clearance is obviously not respected. Is it critical ? \$\endgroup\$
    – chris
    Jun 24, 2016 at 3:23
  • \$\begingroup\$ I'm not entirely sure I understand, I would need to see the design and the components that aren't respecting the clearance, but I'll take my best guess: If you run the design rule check with the components you think are too close to the microstrip, it will probably return errors. You will need to move the components away from the antenna manually -- Altium will not reposition components or tracks to fix clearance problems. You may only have the clearance rule checked on the "batch" check (design rule check). You can set it to "online" to have it show you immediately if you're breaking a rule. \$\endgroup\$
    – DerStrom8
    Jun 24, 2016 at 11:58
1
\$\begingroup\$

In the PCB preferences tab there's a "preferred trace width" setting, this allows you to set custom widths that you can pull up by hitting shift+w while routing. By setting a "preferred width" to the correct microstrip width, you can route a microstrip at any time from any pin without needing to set a rule. This trick works just as well for differential traces too, although Altium seems to keep using the minimum spacing whatever the trace width.

\$\endgroup\$
2
  • \$\begingroup\$ I know how to change the width, what I don't know is how to set the distance between the strip and the ground pouring. \$\endgroup\$
    – chris
    Jun 22, 2016 at 5:24
  • \$\begingroup\$ @chris Ah, you'll probably need a custom rule then, I can only speak for the 2016 version, but the Rule Wizard is reasonably good (you can do it manually, but the wizard's easier), you can set a rule for a specific net, that's probably the most effective way as you only have a few nets that need a microstrip. You could also put a "polygon pour cutout" around the microstrip to keep the ground pour away from the trace, it won't update if you move the trace, but it's probably the fastest solution. Otherwise, find a "coplanar waveguide" calculator as it'll compensate for the nearby ground plane. \$\endgroup\$
    – Sam
    Jun 22, 2016 at 5:29

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.