Equation to make parametric an element

[Anonymous]

Hi guys. Does anyone know how to build a equation to make the circular reinforced steel to the pile to follow the pile length each 8 inches or 20 centimeter for example? I've attached two models that I've been trying to do it.

I'm trying this to make this pile reinforced steel parametric with its length, like the picture attached. Thanks.

 

kelly.young has embedded your images for clarity.

[johnsonshiue]

Hi! I am sorry something is missing in your description. I understand every word but I just cannot visualize what you are trying to do. Have you try using Circular Pattern or Rectangular Pattern? What do you mean by "equation" in this context?

Many thanks!

[IgorMir]

Hi Vick,

If I understand you correctly - you want the reo bars to follow the length of the pilon. Two option are here to start with.

First. if it is one off part - derive the Pilon into the Reinforced Bar file and use its surfaces and parameters to build the reinforcement around it. That way when the Pilon audates - the Reinforcement will follow.

Secon. If you have a family of Poles then iParts and iAssemblies could help.

Cheers,

Igor.

[Anonymous]

Hi. I 'don't know if need an equation. I want to make the circle steel
thing to be dependant of the pile lenght. I mean, in 100 centimeters I
have 5 circler things each 20 centimeters and after I change the length to
200 centimeters, I need to have 10 circle things. But I need that
automized. Let me know if I made myself clear.
I'd like to export to Infraworks and use it there to build a bridge. Thanks
man.

[IgorMir]

Hi Vick,

Try that: create an array and the amount of reinforcing circles in it specify as an equation. I.E. - Length/Space. 

Cheers,

Igor.

[johnsonshiue]

Hi! Then it can be done very easily. Inventor parameters are expression based. This means that you can use one parameter to drive another just like writing an equation. If you cannot figure out, please feel free to share an example here (Inventor files). Forum experts can guide you through the needed steps.

Many thanks!

[j.palmeL29YX]

Is this what you are looking for? (Attachment in IV 2015 format).

Change the value of the parameter "Heigt" and see what happens.

cadder

[Anonymous]

Hi Igor. Thanks for answer, I've tried, but I couldn't place the spacing
that I wanted. And idk why this software creates the double amount of
arrays that I wanted as the picture attached. I'm a very iniciant user.

[Anonymous]

I've attached two files. One is the cap that I'll use to apply on a column bridge. 

The other one "part3" is the pile file. 

[IgorMir]

Hi Vick,

I had a look at your files. If you had IV2018 it would be simpler just to send you a fixed file. Maybe someone with IV2017 can help you out. Otherwise I will have to write you a book on Inventor's Basics.

Best of luck,

Igor.

[SBix26 · Accepted solution]

Here is an Inventor 2017 part file that may help you get the results you want.

I created the pile first (the concrete part).  Then I extruded the longitudinal reinforcing steel as a new solid and used Circular Array to multiply it by 4.  Then I created one ring at half the intended spacing from the bottom, and multiplied that ring using Rectangular Array, with the number of instances equal to PileLg / RingSpacing - 1 ul.  Last, I used the Combine Bodies tool to subtract the reinforcement body from the pile body.

This leaves your part file with two solid bodies: one is the concrete portion, the other is the reinforcing steel.  If you resize your pile, the reinforcing follows.  If you wish to make each piece of reinforcing steel its own body, just use the New Solid button for each pattern operation instead of Join.

Hope this helps,

---

Sam B
Inventor Pro 2019.1.2 | Windows 7 SP1
LinkedIn

[Anonymous]

Thanks! Thank u so much. It'll help me a lot at my university.