Setting Boolean as key

[daan.marijnen]

Hi forum,

I'm stuck on something. I've made a parametric model of a electric motor.

Theres 3 user inputs needed to form a final configuration;

Power x [kW]

Flange size x [mm]

Brake [y/n]

I've set keys to power and flange size, these work fine. But i can't set a key for the brake option for some reason.

I've designed it as follows;

The brake options decides the length of the backside of the motor, so i've made a boolean for brake, true or false.

Then i have the total length of the backside of the motor = waaierkaplengteresult 

I've made a rule;

Now when i use the boolean in my parameter list it all works fine, the model adjust according to the parameters i have set.

But for some reason i cant find the boolean in the tree of when i want to create an iPart, see picture below

Both the power and flange size are there, aswell as the lengths, but not the boolean?

I guess im either looking in the wrong place (less likely), or the way i've designed it is simply not the way it's supposed to be used (more likely haha). I'm a bit of a newbie when it ilogic etc. Any advice or tips are welcome.

Thank you in advance!

[johnsonshiue]

Hi! Unfortunately, iPart does not support Text or Boolean parameter on the author table. I think you will need to workaround it by using a numerical parameter but limit it to 1 or 0.

Many thanks!

[daan.marijnen]

I have adjusted the boolean to a multivalue numiric value; 0 ul and 1 ul (represents no brake or brake).

I adjusted the rule and it works fine inside my iPart, i can also set a key on it so that's a step of progress.

Now when i open a assembly and insert my iPart, i see the key, but it only gives me 1 option, either 0 ul or 1 ul. Depending on what i set it to last inside my iPart before saving, it makes sense, but thats not what i want to achieve

I want to be able to pick freely in my assembly between 0 ul or 1 ul, any tips on how to achieve this?

[johnsonshiue]

Hi Dann,

Let me ask you what exactly you are trying to do. It sounds like you want to use iLogic rule to drive iPart members. Is that true? If yes, I would say it can be problematic. iPart was designed to create library components. It is not meant for on-the-fly configuration or being driven by other components. The only driver to an iPart member should always be the iPart factory and the table within. 

If possible, please share the files here so forum experts can take a look and suggest the best course forward.

Many thanks!

[Daan_M]

Hi Johnson,

Firstly thank you for taking time to help me out. The advice is greatly appreciated and helps my understanding of the software. Before your reply it was indeed my goal to drive iPart parameters with iLogic rules. But if this is not suggested, i will find another solution.

If i understand correctly, i should not drive iPart parameters with iLogic. But it should be fine to drive iPart orientation/placement with iLogic inside an assembly? So as long as i don't toutch the parameters in partfile itself it shouldn't conflict

I have added the file for your referance, you can see inside the parameters i've added a user parameter 'Remoptie' multi-value numeric value (either 0ul or 1ul) to be used in iLogic to change the length in case of a brake. This works fine inside the iPart file itself, i can switch between 0ul and 1ul and it changes length, but it conflics inside an assembly since excel columns only takes one value.

It wouldn't be too much of a proble to copy the entire excel table and duplicate it while only changing this value, but a nicer solution is always welcome.

For the record, i'm a student and by no means expert in drawing haha. 

[johnsonshiue]

Hi Daan,

Yes, absolutely. You can drive an iPart member's orientation and position in an assembly using iLogic (just like doing it manually). But, you should not try to alter author table content using iLogic. There is a reason why the iPart/iAssembly was designed to create library components, which rarely change.

You have to clearly understand the driving and driven relationship between the factory and the members. Otherwise, you will run into troubles.

Many thanks!