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Multiple-cut section views in drawings

abugoci
1-Newbie

Multiple-cut section views in drawings

I'm not entirely sure what to accurately call these, so I haven't had much luck in finding help creating such. At the moment, I'm working to take 2D AutoCAD drawings and turning them into 3D Creo Parametric 2.0 models as well as to recreate the drawings in Creo. In particular, I'm floundering on how to make more complex section views display in my drawings.

Attached is a simplified ref of the original AutoCAD views I'm trying to replicate. I can cut it like the model via an actual extrude but I can't figure out how to get a view looking flat at both cut faces at once. I've also tried to create a xsec with two datum planes in the model itself to then put on the drawing as a 3D cross section, but at that point the view doesn't display the two cutting planes as flat, instead displaying the angled side as coming out of the page and as such a portion of the outer surface is displayed and any attempt to dimension on the view is rendered skewed and worthless.

As an additional little question, where's the option to exclude a part from showing as cut in a cross section of an assembly drawing? With cutting a cylinder I'd like to leave the piston rod fully displayed but cut through all other components.

Any pointers into the right direction for what I'm overlooking would be much appreciated.


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1 ACCEPTED SOLUTION

Accepted Solutions
dschenken
21-Topaz I
(To:abugoci)

You are looking to create an Offset section. It will prompt you to make a sketch of the path the sectioning plane will take. This is not the same as a Planar section with an Offset Datum.

In the drawing you select the crosshatch and Properties. One of the choices is to Exclude the item from the section. You can either click Next/Previous until the section lights up on the item, or I think Select is available for you to pick it directly.

It won't change instantly; it will just not crosshatch it. You'll have update the view or repaint after you are done with the Properties.

View solution in original post

6 REPLIES 6

Create an offset section, menu picks are found in the attachment.

Go figure it's an option I haven't tried yet. Seems like a silly name when it does so much more than merely be offset...

dschenken
21-Topaz I
(To:abugoci)

You are looking to create an Offset section. It will prompt you to make a sketch of the path the sectioning plane will take. This is not the same as a Planar section with an Offset Datum.

In the drawing you select the crosshatch and Properties. One of the choices is to Exclude the item from the section. You can either click Next/Previous until the section lights up on the item, or I think Select is available for you to pick it directly.

It won't change instantly; it will just not crosshatch it. You'll have update the view or repaint after you are done with the Properties.

Thanks for the help.

I'm curious how such a thing ended up merely being called an Offset Section because that was nothing like expected.

Using that option though doesn't make the two cuts lay as though the cutting plane were a flat datum plane like my company's drawn it in AutoCAD. I hope Creo's not too smart with trying to keep it looking like a 3D entity.

As for removing an item from the section, it didn't update when I repainted but going in and editing the view's properties made it properly repaint alright. No wonder why it wouldn't go for me earlier.

dschenken
21-Topaz I
(To:abugoci)

It will look better on the drawing when you create the section view.

Kevin
10-Marble
(To:abugoci)

In a drawing view you also want to use Full(Aligned) for the section properties to make section look like you first picture.

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