Multi Split / Multi bodies in less clicks

[NachoShaw]

Hey

ok imagine a chessboard pattern with 20 x 20 array of rectangles (400 squares).

i need to split this into individual bodies (each body being unique).

How can i split this so that each piece is a separate body without using 400 features to split it up? Is there a method where i can just split all into individual bodies with a sketch in one go? Or, select a body and make independent?

Thanks

Nacho

[SBix26]

If the 20 x 20 array is a rectangular pattern, edit the pattern and change the options to Pattern solids and Create new bodies.  Then you will have 400 separate solids without all the trouble and repetitive stress of splitting each one.

Hope that helps.

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Sam B
Inventor Pro 2019.1.2 | Windows 7 SP1
LinkedIn

[NachoShaw]

Hi

they are not a pattern. in my real part, they are all slightly different sizes each making a larger pattern when grouped together so, each panel is unique and i cant array them im afraid

[SBix26]

Can you post pictures or files?  How are these created to begin with?  What version of Inventor?

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Sam B
Inventor Pro 2019.1.2 | Windows 7 SP1
LinkedIn

[NachoShaw]

Hi

I can post an image later when i get to my machine. In the meantime:

I import 2 CAD sketches (Plan & Elevation)

Line them up with the same center point etc

Extrude the elevation section (as it has undulations of a waved panel)

Extrude cut the plan through the elevation (to give me my outline, like a cookie cutter with 1/4" gap between each proposed solid body)

I then need to separate the main solid body into individual bodies.

The above process should results in about 200 individual solid bodies that i need to separate and export as part panels. Currently, i have added a plane to each edge (at the 1/4" gap) which gives me a ton of planes. Then i have to split each one individually which gives me a ton on splits.

I know it would be awesome to simply select a body entity and select say 'Make independent' or 'Separate All' but i doubt anything like that is available. 🙂

Nacho

[Tom_Sturtevant]

I’ve got two ideas on this.  Neither is totally clean but they may save you some clicks…

Idea #1:

If the “cookie cutter” profiles in the Plan sketch are identical or at least identical within tolerance of the 1/4” gap (and if I’m correctly understanding your description!) you can:

+ create an initial extrusion of one of the plan sketch “cookies”  (excess length will be trimmed later)

+ use pattern of solid to get 200 bodies

+ cut all bodies with your Elevation section with a single Extrude Cut (browser selection of the bodies will support SHIFT+Select so you don’t need 200 clicks – but it will be SLOW picking up 200 boides)

+ (if needed) cut all bodies again with your plan sketch to enforce the 1/4“ gap.

Idea #2:

This involves converting each “lump” (“cookie”) to a surface, then using Sculpt to convert the surface back to a solid.  Definitely not a clean workflow but maybe less clicks (and certainly less workplanes) than using split.

+ start with your single solid consisting of 200 “lumps”

+ Use Copy Object to convert one “lump” to a surface

    3D Model > Modify > Copy Object.   Check “Face” selection.  Check “Composite” output.  Select all faces of one lump.  Apply.  (Hint: if you are viewing at your Plan sketch you can use window select.)

+ Repeat for the other 199 lumps (the surface display will help you keep track of what is left)

+ Turn OFF visibility of the 200 lump solid.

+ Use Sculpt to convert one of the surfaces to a solid.

    3D Model > Surface > Sculpt.  Check the “New Solid” option.  Select one surface.  OK.

+ Repeat for the other 199 surfaces.  (Hint: space bar to repeat last command will help)  Make sure to select “New Solid” EVERY time.  Find the “Inventor Ideas” site and request that Sculpt retains the “New Solid” previous setting and has an “Apply” option.

+ Make sure you now have 201 solids.

Hope one of those will be helpful…

T.0.M.

[tomas.baborsky]

I have also this problem. I have a face and created there some lines and I need to seperate this face into many faces.

So if I understand well, it is not possible? 😄 Huh.....

[johnsonshiue]

Hi! It is possible. You can use Split command and select the line to cut the selected faces. However, if the lines are not forming a loop, you will need to repeat the process for other lines.

Many thanks!