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Introducing Combine in NX 11.0.1

Siemens Creator Siemens Creator
Siemens Creator

Combine is a new feature modeling command in NX 11.0.1. The purpose of Combine is to “combine” multiple sheet bodies. In the example below, three sheet bodies are combined into one sheet body.Three combined into oneThree combined into one

 

Combine is a Boolean. Regions of intersecting sheet bodies are selected to include in the combined body. Regions that are not selected are trimmed.

 

I select a sheet body by clicking a region to include. For example, I click the bodies where illustrated below. The regions I click form the combined body. Think of this interaction as “what you click is what you get.”What you click is what you getWhat you click is what you get

 

It is not always convenient to click on a region to include in the combined body. In the example below, numerous sheets are derived from layout geometry. On several bodies the region of interest is obscured and thus difficult to click. Even when I rotate the view, some regions are obscured.Combine4.jpg

 

If I multi-select, with a rectangle gesture for example, Combine will attempt to find a logical volume and automatically select the regions necessary to enclose that volume. The product of this example is a solid body because the regions enclose volume.Multi-selectMulti-select

 

With the Combine interface, I can manually select regions if I need to include multiple regions of a single body or if my click point on the body was not on the region I actually wanted. In the example below, I need to select two regions of the cylinder.Multiple regions of one bodyMultiple regions of one body

 

I can choose if the regions I select are included in the combined body or excluded from the combined body with the “Keep” or “Remove” option.Combine dialogCombine dialog

 

Details to know:
  - Bodies must physically intersect to find regions to combine.
  - Combine always creates a new body – the originals are not modified.
  - Combine is applicable to sheet bodies, not solid bodies. For solid bodies, use the Unite command and select regions to keep or remove.
  - Find volume occurs automatically with multi-select. If you individually select bodies by clicking regions, you can manually execute find volume by clicking the button on the dialog.

 

Eric
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