Help needed setting up iLogic Part

[RobertT1986]

Hi,

I'm fairly new to inventor. I've certainly only dabbled with derived parts and never with the iLogic functions.

I am designing fixture which requires a stack of 30 1mm thick laminations. 

I want to create 30 unique profiles with the highligted circle cut features rotating counter clockwise 1.2 degrees on each profile The other features stay the same. When the profiles are stacked up there will be a 36 degree skew over the stack, as shown on the solid model. I am looking for the easiest way to generate these 30 profiles automatically and be able to parametrically change the size of the hole and apply to whole group should I need to at a later date.

Any tips on where to start would be very helpful indeed.

Many Thanks

Robert

[dkatz]

Hi Robert,

I'm not sure you even need to use iLogic.

If you set up an ipt with your sketch there. Then add a parameter "Skew Angle"  to control the skew of the entire sketch, you should be able to create an ipart. That will let you make 30 items each with their own skew angle.

Then, you'd just assemble them in a .iam file and lock all their XY planes together

Does that work?

Thanks,

Dave

[RobertT1986]

Hi Dave,

This sounds very hopeful, I'll look into iParts this morning and give it a go.

Thankyou for your help!

Robert

[RobertT1986]

I'm sure i'm doing something very silly here.

I'll keep on plugging away and reading up on iParts.

But in the meantime if anyone has a quick answer on what I may be doing wrong here It would be much appreciated.

I've uploaded a jpeg showing what happens each time I try to create the parts.

Thanks

Robert

[JDMather]

Can you attach the *.ipt file here?

Have you named the parameter the same (you don't actually show it in the screen shot, but you have typed "skewangle" and "Skewangle").  These would be seen as two different variables by Inventor.

[RobertT1986 · Accepted solution]

All sorted now.

After reading through a few threads I found the problem was I didn't have MS Excel installed. Only OpenOffice, which it didn't like.

60 day trial of MS Excel installed, so that's bought me some time whilst I try and convince the powers that be that I need MS Excel to do my job.

Seems crazy that inventor would rely on having to have Excel installed, but there you go.

Thanks all for help.

Robert

[dkatz]

Wow, that's something I hadn't considered...I'm really sorry that turned out to be the case. Everytime I read one of these cases where people run up against some inventor obstacle, I'm imagining some evil troll on the bridge between us and we want, and he is cackling as he blocks the way. (No, I am not calling Autodesk an evil troll - I'm just saying, this is what pops up in my head).

Glad to hear you got the model side of it nailed down, though.

[RobertT1986]

Right, I'm there with the design on this one now.

Just one more question. The 30 unique profiles are to be lasercut. To help identify them the lasercutters can etch a number onto each one. but that number needs to be on the .dxf file we send them. Basically each part needs to assigned a number #1-30.

Is there an easy way to set up an extruded sketch or similar that will sequentially increase on each iteration of the Ipart? 

Or is it doing to be more straightforward to manually put it in using autoCAD, before they are sent.

All advice welcomed.

Thanks

Robert

[dkatz · Accepted solution]

Hello again!

Looks like you could continue to take advantage of the iPart table.

Create yourself a parameter called Item_Number (Or whatever you like...note the underscore in the name - you can't have spaces). Change the units of this parameter to be ul (or unitless).

Then create a new sketch on the face you want the text to appear. In the "draw" section of the ribbon, there's a command called "Text". Click that. When you get to that dialog, you need to select User Parameters, Your parameter name, And the precision (no decimal places in this case).

Then click the d0 button to insert your value. I'd also center it vertically and horizontally, because I'm me. Click Ok to add the text to your sketch

Constrain your text like any other sketch. Then use the emboss tool. Select the text as the profile, Select the "Engrave from face" option, and enter the depth of your cut. One note about cut depth...if you are Rapid prototyping these, make sure it's greater than the minimum feature allowed on that specific printer. Otherwise, it might just get ignored.

Now go to your iPart table and add the parameter from 1 - 30 in your table. Your parameter may be listed in the "Other" section instead of underneath your extrude feature.

Let me know if that does it for you.

Thanks,

Dave

[RobertT1986]

Perfect! Exactly what I wanted to do.

Thanks so much

Robert

[dkatz]

Awesome! It's my pleasure.