Rope pulley system

[Inventoruser24]

Hi. I've got this sort of rope-pulley system. A handle, a weight and an adaptive rope that goes around three wheels.
The goal is when the rope at the handle end is pulled (extended), then the rope in the other end will go up (shortened).
At first I managed to do this within the sketch, pulling one sketch line made the other sketch line go short. But when I exit from the sketch everything was fixed. However, now this doesn't work in the sketch either.
But also I'm not sure where to put constraints that can be used for "drive" later, and where to constrain the parts. I believe this is the main issue. I tried many hours and watched some youtube videos too but this didn't do it. Any advice would be greatly appreciated.

[CCarreiras]

Hi!

You're expecting we can find a solution only looking for the images?
How the parameters are related? what constrains used?... etc etc.

Share the model and we will try to find the issues.

[Inventoruser24]

My apologies, I have shared the model in the main post now. Since it's far from finished and I've been experimenting with it some I'm afraid constraints or parameters in it wont make much sense.

[kacper.suchomski]

Hi

There are 2 ways:

1. Adaptive line sketch. The sketch must be adaptive to the projection of the active component geometry. The passive element must have a standard constraint with the other end of the rope.
2. Parameterization - you can combine the length parameters of individual (straight) rope segments using iLogic to create the equation that the straight section = the height of the pulley axis - the height of the active element (position) - the height of the active element (dimension). The passive element must have a standard constraint with the other end of the rope.

In both cases, the sketch must contain an equation that determines the length of one straight section from another, and the passive element must be connected to the rope by standard constraints.

[CCarreiras]

Hi!

You don't need to do big formulas, you can have the movement purely based in geometry:

[Inventoruser24]

kacper.suchomski, thank you. Would you mind explaining a bit more how number 1 would look like? Very new in this and haven't used ilogic. Earlier in sketch mode I used something like this as dimension: 2600 mm - d11 - d10 - d5 - ( 3 mm * 3,14 ul * 35 ul ). It worked for some time but I still had the issue that when I exit from the sketch nothing can move since everything is constrained. So I would need to have a constrain/mate and "drive" it to see motion. I believe here is the big issue for me.

CCarreiras, thanks for the video. I manage to this in the sketch with the angle like you've shown. But when I exit from the sketch it is all fixed and can't be moved. Is there a way to do the same thing you did but with assembly constraints instead and use "drive"? Replied to kacper.suchomski also I think this would do it, a constraint that I RMB click and choose drive. I havent used Ilogic and forms before. 

Thank you in advance.

[CCarreiras]

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@Inventoruser24 wrote:

CCarreiras,  But when I exit from the sketch it is all fixed and can't be moved. Is there a way to do the same thing you did but with assembly constraints instead and use "drive"?

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The system moves based in the variation of the parameter Angle... and it works well.

If you want to move the system based in another method, you have to explain better what you are really trying to do.

[Inventoruser24]

I can manage the motion/variation of the angle parameter within the sketch, but not outside the sketch.  So how to demonstrate how everything works together with other parts if I only have the motion within the sketch? If iLogic is the way then I'll try to learn it.

[CCarreiras]

In the assembly:

In parameters chart create The parameter "ANGLE" (select "deg" as unit).

In the part, rename the angle parameter from d1* to "ANGLE" (* as an example... could be other value in your case: d8, d10, d5, etc)

In the assembly, open the iLogic browser and create the rule to connect those parameters (this way, when you change the parameter in assembly environment, it will change in the sketch).

The rule is:

Then, in assembly environment, create a FORM and add the ANGLE variable.

Change the input as SLIDER, instead of Text Box.
Set the minimum and maximum value for the ANGLE value you need to work without causing errors.

Click ok... and now you have a slider to change the ANGLE value and see the result on the fly.

[Inventoruser24]

Many thanks for your help, I will try this. Wish you a great day ahead.