Forums » CircuitLab Support Forum

Hi all! This is my first circuit and i'm trying to understand if i have a mistake with placing the right symbols (power supply?) or i have a problem with the actual circuit. this circuit supposed to create a triangle wave and square wave with rate control (i copied it from a device service notes and checked few times for mistakes). while running the DC simulation i can not test any point on the circuit. can you see any problem that can cause that?

Thanks in advance and sorry for the bulky execution...

https://www.circuitlab.com/circuit/q8wtsz/mod-osc/

@oneoff7,

Welcome to CL.

You have a few minor typos in the schematic.

The "rate" pot probably has to be called something that the CL simulator recognises as a resistor such as RV1 or simlar (though in fact calling it "rate" is OK because it begins with R).

The "rate" pot value should be 1M for 1 Megohm. In CL, 1m = 1e-3 Ohms.

The integrator cap round the LM741 has a spurious suffix: you don't need to add "F" at the end of a cap value (or H to an inducotr etc.). CL adds the suffix for you.

You cannot get an answer to a DC analysis on aqn oscillator because it has no stable DC operating point.

Try running a transient sim to see if it works.

I had a quick go but it seems to struggle. You could try simplifying the circuit: take out the duty cycle adjustment diodes in front of the rate pot. Strip it down to the bare functional circuit, get it running then build the trimmings back in.

thanks, what are the default values of the pots? would it be the max values? also if i want to use pos. and neg. power can i do it in a more efficient way as opposed to connect an actual wire to each point on the circuit .

Double click on the pot symbol.

The 'K' value in CL pots is the proportion of rotation. 0.5 = pot half way round, i.e. TAP is at mid position between A and B. 0 means fully at one end, 1 means fully to other end. How you interpret which 'end' is which depends on how you connect pins A and B of the pot!

To connect nodes together without discrete wires just attach the same net label to them.

About Wires and nodes

If you hover your mouse over the end of a lead of a component that you have placed on the schematic a large, light grey dot will appear right at the end of the wire.

That is the (only valid) connection point for that component lead. Also referred to as a Node:

https://www.circuitlab.com/docs/the-basics/#nodes

If you Left-click and hold on that grey dot then drag the mouse cursor, a wire will appear.

Drag it to the next node you wish to join.

If you need to turn a corner, let go and then repeat the process on the node dot at the end of the wire you have just drawn and drag at right angles.

Note that you can also join nodes just by attaching a label to a node and then attaching a new label with the same name to another node. Those two nodes are now connected exactly as if you has drawn a wire between them:

https://www.circuitlab.com/docs/the-basics/#named_nodes

You can also draw a wire by clicking on the "Wire" button on the left hand palette then left-click and drag and release on the schematic.

To repeat a placement press shift before you click on the component you wish to place.

However, you must be consistent in your labelling:

https://www.circuitlab.com/forums/support/topic/86m9393x/bug-report-inconsistency-in-using-net-label-as-a-voltage/

Note also that CL assigns arbitrary but sequential node names to unlabelled nodes.

This can lead to very confusing results where node names are used in expressions for arbitrary sources and plot expressions.

Suppose you have a circuit with 17 nodes then you replace a resistor with a piece of wire.

Your circuit now has only 16 nodes. Suppose the node you removed was Node17.

Suppose you then add a new component in a different location that then adds a new node (by inserting a resistor in a wire for example). The new node will be auto-labelled by CL as Node17.

If you now add the first resistor back in it's original location. The node that reappears will now be auto-labelled Node18 and not Node17 as it was originally.

More complex editing makes a more comprehensive mess of the CL assigned node names.

If you put node name labels on all the nodes you are interested in then they won't change numbering or flicker in and out of existence as you edit your circuit. They will then always be valid in your expressions.

You can set up explicit voltage sources for the power supplies in CL or create an implicit supply using a node or net name. For example, the +1V or +1 node label invokes an implicit 1V source:

https://www.circuitlab.com/circuit/a5bzf7/good-netname-and-a-free-voltage-source/

However, in:

https://www.circuitlab.com/circuit/96br67/bad-net-name/

CL throws an error because the explicit 1V source, V1, is then in parallel with the implied source created by the node label.

thanks a lot for the details!

I'm still having issues with some simple circuits which actually works on the breadboard and in circuit lab I'm still getting "error infinite value"

what does this message mean ? where should i look for mistakes? for example this simple LFO: https://www.circuitlab.com/circuit/5p26fd/mfos/

or this one: https://www.circuitlab.com/circuit/aya8jd/new-miss10/

(copied straight from the designer schematics )

i'm not sure what i'm doing wrong...

Scaling factors in CL are case sensitive.

In:

https://www.circuitlab.com/circuit/5p26fd/mfos/

you've typed C1 as "0.1U". If you replace it with "0.1u" then a time domain sim will run but the circuit will not actually oscillate.

That's because you need to kick it into life.

To fix this, try putting this expression into V1:

15*(1-exp(-T/10u))

and/or this into V2:

-15*(1-exp(-T/10u))

This should also fix:

https://www.circuitlab.com/circuit/aya8jd/new-miss10/

For more on this trick, search CL for:

oscillator-startup

initial-conditions

startup

:)

Thanks a lot that sorts it out for me... cheers