Jump to content

LS Research TiWi-R2 Module PCB/Booster Pack

Recommended Posts

Thanks Zeke,


If I understand correctly:


I should add a copper pour on top underneath the module, bottom has one already (in blue), or do you mean the whole bottom?

I should add more vias there


Im not sure if I understand

If you ground the H. E. double hockey sticks out of the board then it will work well

I had trouble making that contact detail work like the drawing, so I improvised with those 4 pads that fan out to the proximal vias,


I was under the impression the power planes were for heat sinks, much like the HT case IC's


Thanks again for such a quick reply. KB


p.s. I have improved it as you suggested, but i cannot upload for some reason, i will try later.

Link to post
Share on other sites
  • Replies 36
  • Created
  • Last Reply

Top Posters In This Topic

Top Posters In This Topic

Popular Posts

Don't feel bad!   Making mistakes is perfectly normal and they are perfectly acceptable. Anyone who criticizes you for making a mistake deserves to be knocked to the ground!   Making mistakes mea

Learn from your mistake. For a first job, it come out well.

Ah nuts. I'm 200 miles away from home and all I have is my iPod touch. It's useless for checking layouts.   I'll be back home tomorrow and I'll check it out then.   Hopefully Designspark is easy

Posted Images

The four features that are under the chip and on the top-side of the board, are just exposed copper pads. They connect to ground.


They have something called a thermal relief which is a cutout in the copper around the exposed pad. Normally, this is done on through-hole vias tied to ground. The thermal relief gives the technician a fighting chance at desoldering the through-hole component.


If it were just solid copper then it would take a 1000 Watt soldering iron to get enough heat into the joint to melt the solder. By that time, the component would also be liquid.


So, I would have to say that the manufacturer wants the thermal reliefs there so that the component will actually solder down to the board during the reflow process.




And now I want to ask you how you're planning on soldering down this device? Toaster oven?

Link to post
Share on other sites

:thumbup: :thumbup: :thumbup:


That looks perfect to me.


One more thing though. I just noticed that the antenna track needs some buffing. It's got to be made into a 50 ohm transmission line.


1. Extended the bottom side ground pour so that it is beneath the antenna track.

2. Place ground pours on along the left and the right side of the top side antenna track.

3. Place a hedge of vias along the left and the right side of the top side antenna track.

4. Make those vias connect to the bottom side ground pour.

5. The antenna track width should be 0.010".

6. The spacing between the antenna track and the top side ground pours should be 0.010". This will make a 50 ohm transmission line.

7. Place an approved RF connector footprint at the board edge so you can connect an antenna to the module. I suggest an SMA connector. Either this or this would be fine. It's up to you.



Is this just a breakout board?

Link to post
Share on other sites

Oh! I just noticed something else that I would buff. You need a really beefy ground system!


On the left side of the board, bottom side, you have a spindley little ground track connecting center ground pour to the left side pins. That will never do.


You should make the ground tracks as wide as possible. Say 0.030" and whatever width you can route between the vias. If you can, you should lay down more beefy ground tracks between the center ground pour and the left side ground pins.


Try laying horizontally the thickest ground track you can between the center ground plane to the top-left ground pins.


Make sense?

Link to post
Share on other sites

I like the complete bottom side ground flood. That will work well.


By the way, is the bottom side ground plane connected to the four pins of the SMA connector using thermal relief pads? Every pad connected to the ground plane should be using the thermal relief pad (for reasons previously noted).


I'm having difficulty knowing what is happening on the top side around the antenna track. I can see the vias lined up like a hedge. Are they connected to a top side ground plane as well? They should be.


Could you extrude the top side ground plane under the module upwards along the antenna track?

It will then connect the vias to the bottom side ground plane.



I can see it now. This is going to be an excellent RF clean board. Good work!

Link to post
Share on other sites

Hi Zeke, thanks for the continued attention.


Please check this out:




I think I included everything you mentioned. It is hard to see the vias on the image, but they are plated. This has caused me a little confusion. I assume "plating" the vias will connect the two ground planes. As an example, the 4 pads in the top ground plane. They are specified as "exposed copper", and i take that to mean a pad with no plating. The other pads for the module I imagine are "plated" meaning they will be soldered on?? Why would the ground plane pads not be plated?


Thanks. KB


it will ultimately do something like this:



Link to post
Share on other sites

Yes. Much like the ProFLEX PCB in the picture above but 2x2". I did not do much with the connections, as I am still trying to get a better understanding of the module. The LSR datasheets are simplified, and do not provide much guidance. My first concern is the 1.8V VIO. There is some mention of signal translation.



Link to post
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

  • Create New...