i-logic Forms - How to include parameters from a sketch

[hristo.hristovMK259]

Hi,

I have an assembly. Fully constrained. A crane, that can change the slew and luff angles, and moves the hook up and down. (rotational and axial movements). I can easily create a i-Logitc Form and have a nice window to put all of the inputs.

However, when I create a sketch then that sketch goes higher in the hierarchy and I cannot use my assembly anymore. I want this sketch to be also included in my i-Logic Form when I change angles, positions etc. but I cannot. Any suggestions how to deal with something similar? 

So, all assemblies (Main Crane, Aux Crane, Deck Crane, Gangway etc) work fine in an i-Logic Form. As soon as create this sketch that I also want to be able to use in my Form it ruins it. Any other workaround of how to include something similar to that sketch? See the things in Blue colour that I also want to be able to have in my Form (radius and relative angle (highlighted as 50 deg and radius 100 m highlighted in blue)

ATTACHED SCREENSHOT (I used water colour style to hide sensitive info, sorry if it looks messy)

[WCrihfield · Accepted solution]

Hi @hristo.hristovMK259.  If you want to be able to control sketch dimensions from within an iLogic Form, then you will first need to know which Parameter objects are controlling those sketch dimensions, then you will need to add those Parameters to your Form using the Form Editor dialog.  Within the image you posted, I can see that you have the 50 degree angular dimension selected, because the small Edit Dimension dialog is showing near your mouse cursor.  Within that small dialog, you can see the name of the Parameter "d130" that dimension is referencing.  That will be a ModelDimension, and it was likely automatically created for you the instant you created that sketch dimension.  When those types of Parameters are automatically created, they are given automatically generated names using a built-in naming system, and pretty much always start with "d".

There are several options for what you could do next here.

• One option: (Two possible ways)
  • Go into your Parameters dialog and rename that ModelParameter named "d130" to something more meaningful, so you know which one it is going forward.
  • Or, right within that small Edit Dimension dialog, you can enter something like "MyAngleParam = 50 deg", where it currently shows 50, and that will rename the ModelParameter directly for you.
• Another option:  You could create a new UserParameter in your Parameters dialog with a meaningful name, then copy its name, then paste the name in the Equation field of the ModelParameter named "d130", so that the UserParameter's value will drive that ModelParameter.

Once you have done either of those steps, you can now add either the renamed ModelDimension, or the new UserParameter into your Form, using the Form Editor dialog.  I personally prefer the second option with the new UserParameter, because they are permanent, while the ModelParameter will disappear if you delete the dimension.

[Curtis_Waguespack · Accepted solution]

Hi @hristo.hristovMK259 

I typically try to avoid using sketches as inputs for changes to angles because the angle dimension can flip on you and go in the negative direction.

Generally, when we are using a form to control an angle like this it is better to create a workplane and drive the angle of the workplane instead.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[hristo.hristovMK259]

@Curtis_Waguespack Could you please explain how exactly would you control the positioning of that 50 deg angle and how can you control the radius in a Form? Working Planes, how exactly?

Please note that I have done this for the crane itself, luffing, and slewing angles, but this is more like the actual position of the cargo on the ground (as manual input in the Form)

In addition, when I plot this, I would like to be able to see this in the Sheet and dimension it (for example, R50 m, angle 50 deg etc) in 2D plan view and add the rest of the dimensions on the sheet.

I hope I am clear enough, as it is not so straight forward to explain it 🙂 

[Curtis_Waguespack]

@hristo.hristovMK259  what version of Inventor are you using?  Inventor 2022, Inventor 2023, etc?

It might just be easiest for me to provide an example.

[hristo.hristovMK259]

Hi again,

Inventor 2023.

Basically, this sketch is a separate thing from the crane but also shall have the possibility to be included in an iLogic Form for a different purpose.

[Curtis_Waguespack]

Hi @hristo.hristovMK259 

See the attached example files.. The angle controls the work plane angle in the assembly, and the components are constrained to the plane.

If we try to use a dimension in a sketch for this, often times when we go to zero, Inventor gets confused and solves for the wrong direction, because sketch dimensions don't have a negative, and therefore our sketch angle can flip and become unpredictable. 

Using work planes eliminates this.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[hristo.hristovMK259]

Thanks a lot, I will look into it tomorrow!