Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronic 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

[SOLVED] Bipolar Dac I-V converter and LtSpice simulation

Status
Not open for further replies.

little0192

Newbie level 5
Joined
May 26, 2016
Messages
10
Helped
1
Reputation
2
Reaction score
1
Trophy points
3
Activity points
117
Hi,
I am designing a +/- 10V output DAC board using a current output DAC (PN : AD9767ASTZ).
So I am already using a reference design for a Evaluation Board from here. The board can be configured for the different outputs. I am interested in the 3rd type for making +/- 10V signal output.
1593510562909.png

My first question is why they haven't used the 50 ohm parallel termination on the IoutA and IoutB. How is this series arrangement (in the Figure 9 above) functionally different from the parallel termination. However, In the LTC1668 datasheet the suggested circuit has parallel termination only.
1593510866869.png

Secondly, I am trying to simulate the circuit in the LTSpice to understand it better. But I am not getting the expected result. Can anyone guide/tell me what I am missing in the simulation? I am using a current source to emulate the Complimentary current output of 0-20mA.
I am attaching the LtSpice Simlation file as well. Thanks🙏.


1593510407778.png
 

Attachments


BigBoss

Advanced Member level 5
Joined
Nov 17, 2001
Messages
4,740
Helped
1,434
Reputation
2,866
Reaction score
1,298
Trophy points
1,393
Location
Turkey
Activity points
28,635
Try to use 2 Current Source that are connected in symmetrical configuration.
Sweep current value from 0-10mA for each..
 

    little0192

    points: 2
    Helpful Answer Positive Rating

dick_freebird

Advanced Member level 5
Joined
Mar 4, 2008
Messages
6,753
Helped
1,990
Reputation
3,984
Reaction score
1,815
Trophy points
1,393
Location
USA
Activity points
54,171
If you treat the op amp + R4 as a transimpedance amp
then its closed loop transimpedance is 1K and your
20mA input crest current should make a -20V output,
well greater than the +/-12V op amps can follow. To
this you are also adding 10mA from the VREF (which
would at crest drive you to -30V). What you probably
are seeing, is that only the lowest currents can be
amplified without clipping in the first stage, and the
clipped signal can't be restored by the second stage
offset.

Lower DAC current, or constrain first stage to remain
linear with max DAC current, and make it up in the
second stage?
 

    little0192

    points: 2
    Helpful Answer Positive Rating

little0192

Newbie level 5
Joined
May 26, 2016
Messages
10
Helped
1
Reputation
2
Reaction score
1
Trophy points
3
Activity points
117
Try to use 2 Current Source that are connected in symmetrical configuration.
Sweep current value from 0-10mA for each..
Thank for replying.
I added the two current sources as you said but still not getting the result. Is there any other configuration I can try? Thanks.
1593608751006.png
--- Updated ---

If you treat the op amp + R4 as a transimpedance amp
then its closed loop transimpedance is 1K and your
20mA input crest current should make a -20V output,
well greater than the +/-12V op amps can follow. To
this you are also adding 10mA from the VREF (which
would at crest drive you to -30V). What you probably
are seeing, is that only the lowest currents can be
amplified without clipping in the first stage, and the
clipped signal can't be restored by the second stage
offset.

Lower DAC current, or constrain first stage to remain
linear with max DAC current, and make it up in the
second stage?
yes I am getting what you are saying. If I reduce the current to 5mA then I am getting sine wave-output. But that means that the circuit is not using the full scale current output from the DAC. In the manual they did not mentioned the functionality.
Since this circuit is already verified I think I may be wrong with the implementation of the current output from the DAC.
Can you suggest me what should I try next? Thanks.
--- Updated ---

Try to use 2 Current Source that are connected in symmetrical configuration.
Sweep current value from 0-10mA for each..
Here is the LTSpice file.
 

Attachments

Last edited:

BigBoss

Advanced Member level 5
Joined
Nov 17, 2001
Messages
4,740
Helped
1,434
Reputation
2,866
Reaction score
1,298
Trophy points
1,393
Location
Turkey
Activity points
28,635
There might be some problems in macro-model of the Op Amp.
 

little0192

Newbie level 5
Joined
May 26, 2016
Messages
10
Helped
1
Reputation
2
Reaction score
1
Trophy points
3
Activity points
117
There might be some problems in macro-model of the Op Amp.
Spice model is working fine. I checked with the test jig example.
--- Updated ---

So as I suspected that I am doing something wrong with the current sources. I looked once again at the DAC datasheet and found out that it is a current sink device. That means the IOutA pin actually sinks the current, the current is sourced from the op-amp output.
Also the complimentary output means that when IoutA is sinking 8mA current the pin IoutB will be sinking 2mA for a full scale current of 10mA. See the below image for reference.
1594111028481.png
Now getting clean waveforms.
Input current wavefroms1594111315056.png
Input Current

Thanks, I appreciate the help.
 

Attachments

Last edited:

Status
Not open for further replies.
Toggle Sidebar

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top