Extrude - Cut and Retain

[malcolm_smith]

I would like to be able to extrude through an exiting body as cut and be able to retain the cut material as a new body. This would be handy for sub-dividing a single body into a number of smaller bodies.

To do this operation currently I have to duplicate the body using a rectangular pattern (with pattern distance of zero), then perform a cut extrusion on the first body and a combine extrusion on the second body. This works OK, but it is three steps  and it could be done in one step.

From a UI perspective, implementing this would only require the addition of a check box on the cut and combine extrusion types to retain the cut material. In each case the cut material would become the new body, so choosing either the cut or combine method would enable you to choose which part of the body retains the original body name.

[Anonymous]

there is already this feature i have shown the steps to achieve this

first start with your body as shown

then draw the sketch of the slice you wish to take

click  on slice in the 3d modeling tab

click on the bottom of the three buttons on the left of the window that appears and then select the solid and the sketch in the appropriate

places 

you should get something like this

then move the solid you have out of the way using the modify move command

and the final result should be

hope this helps 

[DRoam]

@Anonymous's method would work in some situations, but probably the easier and more versatile way to do this would be using the Combine tool, which is a little mis-named. It should really be named the "Combine/Remove" tool, because it does both. It can either combine two solid bodies into one, or it can remove the geometry of one solid body from another, and optionally keep the toolbody or remove it. So to do what you want, you'd follow these steps:

1. Create your first body
2. Create the extrusion which you want to be part of your new body, making sure to select the "New Solid" button
3. Click "Combine"
4. Select your first body as the Base, and your extrusion as the Toolbody (because it's what will be performing an operation [in this case a cut] on your first body)
5. Select the "Cut" operation
6. CHECK "Keep Toolbody" so your extrusion is retained as its own Solid like you want
7. Click "OK"
8. Inventor may turn off the Visibility of your second solid. If it does, just go into the "Solid Bodies" folder and turn the visibility back on.

This is a really powerful and versatile method that will work in any situation. It's especially powerful because you can build whatever shape you want, way beyond just an extrusion, for your second body, and still use this method to cut its shape from your first solid. Hope this helps, let me know if anything didn't make sense.

[malcolm_smith]

@Anonymous, thanks, I didn't realise that I could just use a sketch to do a split (even though I've been using Inventor for 15 years). I have always extruded a surface first, which is an extra operation. I have found, though, that split operation is not always reliable, particularly on thin shell bodies. Also, the integrity of the sketch is a bit more important than it is for an extrude operation.

@DRoam, the method you describe is the one I usually use. I just figured that it would be possible to reduce the number of operations. Also, Combine operations tend to make the browser history a bit more difficult to follow and you loose the name of the original body. I agree though that it is a more flexible method than simply using an extrusion.

[DRoam]

I can empathize with Combine making the browser history hard to follow, I've experienced that, too. But losing the name of the original body I haven't experienced. If I do a Combine with "Keep toolbody" unchecked, the second body is swallowed up in the original, as it should be, AND the original body keeps its name. If I do a Combine with "Keep toolbody" checked, BOTH bodies remain AND keep their original name. What version of Inventor are you using?

[malcolm_smith]

@DRoam, I just checked and you are correct. It is the split method I was thinking of which loses the name of the original body. The split method converts the original body name to "Solid"n and creates a new body with the name "Solid"n+1.

[DRoam]

@malcolm_smith, to respond very belatedly do your comment, I definitely see what you mean with the split command. It does indeed seem to eliminate the original solid altogether and replace it with two new ones (one for each side), giving both solids a new name in the process.

This not only makes the name disappear, it also makes all downstream features sick until you tell them which solid to apply to.

It seems it would be much better to let us chose a "master" side which is retained on the original solid, and only create the "non-master" side of the split as a new solid. Then we would still have the original solid with its name, and we would only have to repair features built on the non-master side as opposed to ALL features.

I've created an Idea requesting just that, which you can vote for here: Retain original solid and its name after a Split.

[malcolm_smith]

Thanks DRoam, I have added my vote to your idea.

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[inv.ideareview]

Thanks for sharing your Idea. We use this forum to guide product development and help users in the best way we can, based on voting. We occasionally merge Ideas or archive old ones to keep the forum working properly - it ensures there is room for people to review new Ideas and that the most relevant and meaningful ones can gain votes. We’re archiving this Idea because it's been on the board for well over a year and hasn't received many votes from the community. If you want to raise it again and try to gain more support, you're welcome to do so. We’ve found that pictures and mock-ups can help get concepts across and win more votes from other users. If you have questions or see a connection between this Idea and others, let us know. - Inventor product team (Inv.idea review)