Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

Altium, tinned tracks to carry more current

Status
Not open for further replies.
T

TechGuy

Junior Member level 2
Junior Member level 2
Joined
Nov 18, 2013
Messages
21
Helped
0
Reputation
0
Reaction score
0
Trophy points
1
Activity points
159
Altium, tinned tracks to carry high current

Hello,

I'm designing a motor control board which will handle 3 channels of 26Amper each therefore almost 80Amper the input.
I have never designed a board before to handle such a high current!
What's the best way to design the thick tracks to handle the high current?
Can someone help me how to make the thick tinned tracks with altium?
Is that called HASL Finish?
Do I need to remove the solder mask of the tracks?

Thanks any help would be really appreciated.
 

You shouldn't overrate the effect of thick tinned traces. Tinn specific resistance is much higher than copper. You better use sufficient wide tracks and order PCBs with 70µ (2 oz) copper plating.

I don't believe that Altium has an automatic feature for tracks with removed solder mask, but you can draw the openings manually on the solder mask layer. Hot-air solder levelling is reasonable if you don't have very small SMD components on your board.
 
Tinning the tracks will not achieve what you wan, even if you run solder along them I doubt it will do.
For this current you need external bus bars. (Google them)
Get the free PCB Toolkit from the Saturn PCB website and you can work out the track thickness.
 
Trace width calculation tools can give a basic orientation. But you should also consider the total board power dissipation and acceptable voltage drop. Depending on the application, board overtemperature or voltage drops will be the primary constraint. For copper pours, make a resistance estimation based on sheet resistance, it's about 0.5 mohm for 35 µ copper palting.
 
Unless you give the solder something to stick to, wave soldering a PCB with blank traces (i.e. with removed solder mask) will only result in an irregular and thin layer of solder sticking to the copper. The added conductivity will be small compared to the 70 µm copper and unpredictable.

A PCB isn't meant to carry such high currents because the traces need to be impractically wide to avoid excessive voltage drops. High AC currents also cause a lot of EMI which will affect sensitive components on the board.

If I were you I'd take a look whether it's really necessary to run these traces on the board at all. Perhaps it might be an option to install discrete high current MOSFETs in the application which are controlled by your PCB instead.
 
Do the job properly, using tinned copper is a very old unreliable technique, use the required copper on the board, with the correct weight of copper.
Use 2oz on the outer layers and you will gain extra when the board is plated up (talk to our manufacturer to see how much extra you will get)... Though 4oz is readily available.
Duplicate the power tracks on multiple layers.

Regarding PCB current, cause PCBs are designed to carry current, you just up the copper thickness, track width, duplicate the routes etc etc... We do boards that handle 60 A.
 
Looks like everyone has different opinion! I can't believe that no one out there has never build a high current PCB board. I forgot to mention is for a 12/24 DC Motor, and all the MOSFETs are in SMD.
Can I use top and bottom layers for at least the main 80A track with a lot of vias in between?
Thank you anyway for taking the time to answer.
 
Last edited:

marce said:
Though 4oz is readily available.
Click to expand...
Correct, but none of my manufacturers have 4 oz boards in their standard pool, so those boards quickly get prohibitively expensive for relatively straight forward applications like motor controllers.
 

I design boards to do the job and do the job correctly, cost has to be factored in. Designing a board that does the job is what it is about, if its to expensive then you have to re-think all your options...
I have been doing motor control boards and high current designs for years....
What SMD mosfet's are you using?
How many layers do you have to play with?
Hoe far do the traces have to go from mosfet's to connectors?
Is the current constant or pulsed?
What standards are you working to?
etc. etc.
Where is the power coming from, can you use a plane?
What connectors are you using?
You want to many answers without giving enough information....
Download the Saturn PCB toolkit for one source of current carrying capacity...
 

FvM said:
I don't believe that Altium has an automatic feature for tracks with removed solder mask, but you can draw the openings manually on the solder mask layer.
Click to expand...

It is available in Altium. You need to set Mask expansion to 0mm or more to open solder mask automatically (select entire connection by S,C shortcut and then set the mask value in Inspector panel or do that via rules). When the board will be soldered by paste you can open the track in solder paste layer to get paste on the track automatically.
**broken link removed**

But the effect on current density is really questionable. There are existing special technologies to handle this like heavy copper PCBs. I have not personal experience eith that.
https://www.epectec.com/articles/heavy-copper-pcb-design.html


Petr
 
  • Like
Reactions: TechGuy and FvM

    FvM

    FvM

    Points: 2
    Helpful Answer Positive Rating
    T

    TechGuy

    Points: 2
    Helpful Answer Positive Rating
marce said:
What SMD mosfet's are you using?
How many layers do you have to play with?
Hoe far do the traces have to go from mosfet's to connectors?
Is the current constant or pulsed?
What standards are you working to?
etc. etc.
Where is the power coming from, can you use a plane?
What connectors are you using?
You want to many answers without giving enough information....
Download the Saturn PCB toolkit for one source of current carrying capacity...
Click to expand...

The MOSFET I have chosen are from Vishay, SI7141DP with 1.9 mOhm Rds.
Board layers can be up to 4. MOSFETs from the connector are about 5/6 cm a way. Type of connector is a DRC13-24PA from TE.
The current is pulsed, can I use internal plane for the gnd? Or top layer and some part of the Internal plane for the main Input?
Cheers

- - - Updated - - -

Looks like the tinned tracks are old school!!
Thank you guys for all your comments I'll take in everything.
 

I'll look in detail tomorrow, just going home (well back to the hotel) now.
 

We have had this company come and show us their extreme copper boards. Cost is a little more than alum. clad but for the current you are looking at it might be an option for you.

**broken link removed**

Rick
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top