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Ilogic: Long parts split into several parts (conveyor belt side profile)

t.brosens
Participant

Ilogic: Long parts split into several parts (conveyor belt side profile)

t.brosens
Participant
Participant

I'm working on a generator for a modular conveyor belt. The generator is almost finished, I just have to split the side plates into seperate plates max. 2980mm long for the laser. Is it possible to split the part into several parts by code. (using the extract function or something else).  Bellow an image with a side view of the conveyor belt, an image to explain how to split, and an overvieuw of the conveyor.Isometric_vieuw_conveyor.png

 

Side_view_frame.PNG

 

Side_view_Splitted_frame.PNG

 

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WCrihfield
Mentor
Mentor

Possibly, yes.

If so, would you want to launch the code from the assembly level, or from the part level?

I'm thinking within the code:

  1. Create several offset work planes along the length of the part, at the locations you want to split it
  2. Create 'Split' features, which use those workplanes, and keep both sides.
  3. Use the DataIO property of each resulting solid body to export them to seperate Part files.
    1. You would have to specify what you want to name them and where to save them to
  4. Then, perhaps the most complicated part, reinserting them all back into the assembly, and constraining them where their supposed to be.
    1. This is a whole nother ball game, and only you know the design intent.

Wesley Crihfield

EESignature

(Not an Autodesk Employee)

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Curtis_Waguespack
Consultant
Consultant

Hi @t.brosens 

 

I think you might want to do a replace component with the long one for a shorter one and then pattern the shorter one.  if you can post some simple examples (they can just be basic blocks) that might help others provide some example to get you started, be sure to mention which version of Inventor you're using.

 

here is a link to a past post that shows one method of how to "fill" the pattern in plus a remainder, in case that helps:

https://forums.autodesk.com/t5/inventor-forum/i-logic-assembly-pattern/m-p/3763544#M459819

 

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

 

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t.brosens
Participant
Participant

Thanks for your comment. I think it will work.

In the appendix the assembly with the code and the corresponding part. the code is written in such a way that the part already splits into separate bodies. To save these parts as .ipt is unfortunately too difficult for me. Maybe you can help me? If more information is needed, I would like to hear it.

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tom89Y38
Enthusiast
Enthusiast

@Curtis_Waguespack, @WCrihfield : I'm working together with @t.brosens on the same project. Did you already find some time to check his attachments and last post?

 

Thanks in advance!

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WCrihfield
Mentor
Mentor

Is the Test-plate, a Template part file, that you don't want to save over?

Are you wanting to save each segment length of the Test-plate part off as a seperate part file, or the whole length of the part to a new part file.  Do you then need the code to replace the existing Test-plate part in the Assembly, with the new part file(s)?

Is the Part always going to be divided into 5 sections, or is it 5 sections max (possible to be fewer sections)?

 

Perhaps in the part file, instead of creating one solid at full Conveyor Length, then patterning a plane, then creating a series of "Split" features; you could create a Rectangular Pattern of the first Solid (whose length would be set by a Parameter with a calculation), which ends up at the full Conveyor Length.

You could create a Parameter, which you would use within the Pattern Feature, as the Quantity.

This Quantity parameter ("QTY")would be an Integer, which calculates 'ConveyorLength/Max_Plate_Length', and rounds up to the next whole number.

Max_Plate_Length would remain unchanged, as a limit for the longest allowable length you would consider.

There could be another parameter ("Plate_Length"), which will be used to controll the length of each segment of the part.

This "Plate_Length" parameter would calculate ConveyorLength/QTY to make the pattern equal the exact ConveyerLength.

You would use that "Plate_Length" parameter in your initial sketch of the first Plate.

I believe this may then eliminate the need for the existing iLogic rule, which uses a long series of Select Case, and Feature.IsActive statements.

Wesley Crihfield

EESignature

(Not an Autodesk Employee)

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