Go Back   Home > Forums > >
Home Forums Rules Articles diyAudio Store Blogs Gallery Wiki Register Donations FAQ Calendar Search Today's Posts Mark Forums Read

Chip Amps Amplifiers based on integrated circuits

LM1875, my first project
LM1875, my first project
Please consider donating to help us continue to serve you.

Ads on/off / Custom Title / More PMs / More album space / Advanced printing & mass image saving
Reply
 
Thread Tools Search this Thread
Old 21st December 2007, 03:23 PM   #1
hpl is offline hpl  Sweden
diyAudio Member
 
Join Date: Apr 2006
Location: Sweden
Default LM1875, my first project

Hi all, I'm just about to get started with my first DIY project. I've spent a lot of time reading but I thought I'd just get some feedback on my pcb-layout etc before i get to work.

PSU:
-----
Tx: 120 VA 2x18~
Filtered by anything from 1000 to 6600uf per rail (ill probably start with 3300 per rail As that is what i have available now)

Amp
-----
I'm using the schematics from Elliots site (Project no 72) but want to do my own boards. The layout is made in eagle and I've attached a picture.

Click the image to open in full size.

Do you think the overall layout and specifically the grounding scheme is good, and what about the trace thickness? (signal traces 40 mil, power lines 100mil)

Components:
-----------------
What do people prefer for C1 ? bipolar electrolytic or some other type of capacitor?
Also, any specific concerns about the components in the zobel? film or ceramic?

that's it for now i guess..
thanks,
  Reply With Quote
Old 22nd December 2007, 10:08 AM   #2
Paswa is offline Paswa  India
diyAudio Member
 
Paswa's Avatar
 
Join Date: Aug 2007
I have made the circuit.

I never used this pcb

Thou it seems the pcb is quite good. as it it is from eliott sound projects.

I think 120VA trafo may be boost enough power.

But I'll advice you to get 10,000 uF capacitor per rail coz the 1875 is too sensitive to power humming
  Reply With Quote
Old 22nd December 2007, 10:10 AM   #3
Paswa is offline Paswa  India
diyAudio Member
 
Paswa's Avatar
 
Join Date: Aug 2007
I made it in veroboard and listening now without any problem. so i will advice you to do the same.
  Reply With Quote
Old 24th December 2007, 01:48 AM   #4
Leolabs is offline Leolabs  Malaysia
diyAudio Member
 
Leolabs's Avatar
 
Join Date: Dec 2004
Location: Bukit Mertajam
Send a message via MSN to Leolabs
Make sure u have enough heatsink for the LM1875.This guy sounds good but running hot.
  Reply With Quote
Old 24th December 2007, 10:22 AM   #5
Paswa is offline Paswa  India
diyAudio Member
 
Paswa's Avatar
 
Join Date: Aug 2007
I have a question,

what is the differene between power ground and signal ground.

Will they short?
  Reply With Quote
Old 26th December 2007, 08:36 AM   #6
hpl is offline hpl  Sweden
diyAudio Member
 
Join Date: Apr 2006
Location: Sweden
paswa, thanks for the comments. first, just to clarify, the schematics is from Elliots site, the PCB is not, it is my own layout.

yes i think signal ground and power ground will be connected. I'm still not sure where they will connect though. maybe with a jumper on board or maybe at the central star ground point. I may have to experiment a bit with this...

I've seen lots of people putting a resistor between the actual ground point and the grounding pad on the PCB, not reallty sure why so if anyone can explain this i'd be happy. Is it in order to limit current-sharing between for example signalpath and the powersupply?

i'm ordering parts now and hope to etch my boards soon.

leolabs, i planning to use a shared heatsink for the pair of IC's. the heatsink is roughly 100x75x20mm and specified at 1.5C/W at 50W which should be enough right?
  Reply With Quote
Old 26th December 2007, 02:58 PM   #7
wazzy is offline wazzy  Zimbabwe
diyAudio Member
 
Join Date: Sep 2007
Location: Kadoma
Cool signal ground

hi had some time off recently and have built a couple of chip amps namely TDA 2030, 2040 and 2050, incedentaly the 2050 has same pinouts as the LM1875. you want to have the ground lifted slightly for the signal as this helps to prevent a high current(from your power ground) being carried into your inputs, if you ground your inputs onto the supply ground bad sound, and possibly high DC offset at the speaker may result, with the associated unpleasant side effects, trust me separate tracks and a jumper work really well made four amps so far and background noise almost nonexistant by the way if your power supply is robust enough 3300uf is ok but 6000 always better.
  Reply With Quote
Old 27th December 2007, 03:26 PM   #8
gootee is offline gootee  United States
diyAudio Member
 
Join Date: Nov 2006
Location: Indiana
Default Re: LM1875, my first project

Quote:
Originally posted by hpl
Hi all, I'm just about to get started with my first DIY project. I've spent a lot of time reading but I thought I'd just get some feedback on my pcb-layout etc before i get to work.

PSU:
-----
Tx: 120 VA 2x18~
Filtered by anything from 1000 to 6600uf per rail (ill probably start with 3300 per rail As that is what i have available now)

Amp
-----
I'm using the schematics from Elliots site (Project no 72) but want to do my own boards. The layout is made in eagle and I've attached a picture.

Click the image to open in full size.

Do you think the overall layout and specifically the grounding scheme is good, and what about the trace thickness? (signal traces 40 mil, power lines 100mil)

Components:
-----------------
What do people prefer for C1 ? bipolar electrolytic or some other type of capacitor?
Also, any specific concerns about the components in the zobel? film or ceramic?

that's it for now i guess..
thanks,
Hi hpl,

You've made a good start on the PCB. But there are some things that I think you might want to change, if you do another version. (Note that I have not checked the actual connection topology, versus a schematic. I only looked at the PCB layout issues.)

I would want to get the large electrolytic caps as close as possible to the chip's power pins. You could move the large input cap and all of the other input stuff to the left and/or upward, and put the big electros right up by the smaller bypass caps. You will probably want to leave enough room to be able to use up to at least 1000uF for the electrolytics, there, and maybe even 2200 uF. [The Nichicon low-ESR UHE-series, for example, has a 50V 1000uF model with a 12.5mm diameter (but 40mm height), with 5 mm lead spacing, and also 1000uF (w/20mm height) and 2200 uF (w/35.5mm height) models that have 18mm diameter and 7.5 mm lead spacing. (Their mouser.com part numbers all start with 647-UHE1H, with the remainder being 102MHD or 102MHD3 or 222MHD6.)]

You should probably also give the Zobel's R6 its own separate ground return, back to the star ground point (and probably also connect the speaker's negative terminal to that pad, on this board, so the zobel is directly across the speaker output terminals), which could also help make it easier to move the large caps closer to the chip.

After you build it, you might want to also try soldering a 0.22uF or so film cap directly between the LM1875's power pins, or on the bottom of the board. You could enlarge the traces around the power pins pads, in case you'd rather drill holes for that, instead of soldering directly to the power pins.

Usually, it's a good idea to not have any traces joining with acute angles (i.e. less than 90 degrees). PCB manufacturers call those "acid traps", and they can cause etching problems. So, after you move the large caps closer to the chip, you should probably revise the way the bypass caps' ground traces connect to each other.

You will NOT want to join the signal and power grounds, except at the star point.

I would also try to keep the V+ and V- traces as close together as possible, along with their bypasses' ground return trace, to minimize the loop areas, which should help to minimize field-induced problems. The three power and ground wires should be tightly twisted together, on their way to this board, too. The same idea should also be applied to your signal input and signal ground traces and wires.

I see that you have what looks like a lowpass RF filter for the signal input. Very good. You might want to consider moving it so that its capacitor is directly at the LM1875's positive input pin.

If you want to make the power, ground, and output traces even fatter, that won't hurt anything, either. You could also fatten the signal traces by 50% or more.

You might also want to think about using some type of wire-to-board connectors, and leave room (and matching hole sizes and spacings) for them. Soldering the wires directly to the board often turns out to be very inconvenient, later. Some small terminal blocks might be easy. I'd use two-position ones for the input signal/ground and speaker output/gnd, and a three-position one for V+/Gnd/V-. Examples: mouser.com # 651-1935161 (2 pos) and 651-1935174 (3 pos), which have 5 mm lead-spacing

The speaker ground wire (connecting to Zobel's gnd) and the separate ground wire from there to the star point would have to share a spot in the terminal block, which shouldn't be a problem. But it might be, with some other connector type. You could also just use a three-position connector, there, with the two gnd positions connected by a fat pcb trace.
__________________
The electrolytic capacitors ARE the signal path: http://www.fullnet.com/~tomg/zoom3a_33kuF.jpg
  Reply With Quote
Old 28th December 2007, 01:49 AM   #9
Leolabs is offline Leolabs  Malaysia
diyAudio Member
 
Leolabs's Avatar
 
Join Date: Dec 2004
Location: Bukit Mertajam
Send a message via MSN to Leolabs
Wonder why not put the zobel network directly at the speaker terminal???Save some space on the PCB.
  Reply With Quote
Old 28th December 2007, 05:17 AM   #10
gootee is offline gootee  United States
diyAudio Member
 
Join Date: Nov 2006
Location: Indiana
Quote:
Originally posted by Leolabs
Wonder why not put the zobel network directly at the speaker terminal???Save some space on the PCB.
I have heard of that being done. But I think that the Zobel network should probably be right at the chip's output, in this case.

Here is a quote from the LM1875 datasheet, where, by "output compensation components", they are referring to the Zobel network:

"It is advisable to keep the output compensation components and the 0.1 F supply decoupling capacitors as close as possible to the LM1875 to reduce the effects of PCB trace resistance and inductance. For the same reason, the ground return paths for these components should be as short as possible."
__________________
The electrolytic capacitors ARE the signal path: http://www.fullnet.com/~tomg/zoom3a_33kuF.jpg
  Reply With Quote

Reply


LM1875, my first projectHide this!Advertise here!
Thread Tools Search this Thread
Search this Thread:

Advanced Search

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off

Forum Jump

Similar Threads
Thread Thread Starter Forum Replies Last Post
LM1875 PCB, Which To Use Paswa Chip Amps 281 7th February 2018 08:06 AM
LM1875...how low can you go? Gcollier Chip Amps 7 6th May 2010 03:43 AM
Newbie project - LM1875 or LM3875 redrum.42 Chip Amps 11 19th March 2009 04:38 PM
lm1875 siemensc65 Chip Amps 4 23rd May 2006 03:28 AM


New To Site? Need Help?

All times are GMT. The time now is 01:28 AM.


Search Engine Optimisation provided by DragonByte SEO (Pro) - vBulletin Mods & Addons Copyright © 2018 DragonByte Technologies Ltd.
Resources saved on this page: MySQL 15.00%
vBulletin Optimisation provided by vB Optimise (Pro) - vBulletin Mods & Addons Copyright © 2018 DragonByte Technologies Ltd.
Copyright ©1999-2018 diyAudio
Wiki