inventor versus solidworks

[dho]

i am making a hex nut. the (6) points of the hex will be "turned" down. in solidworks, i make an extruded hex solid first, then i make a circle and extrud it with flip cutting side. then all 6 sharp points of the hex gone. but in inventor.i need to do two circles and extrude cut the area between the two circles. more steps. right?

thanks.

[JDMather · Accepted solution]

Exactly the same in Inventor - use the Intersection command with the second Extrude.

Attach your file here if you can't figure out solution with same number (or fewer) steps than SWx.

[drunknmunki]

For a nut this works fine, but in SWx, if I only wanted half of the nut to be cut using the "flip side to cut" I can just change the distance. Conversely, if I did this in Inventor using intersect, my part is now half as long, and no longer has the uncut portion.
Is there a way to do this without adding extra lines?

[JDMather]

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@drunknmunki wrote:
… my part is now half as long, and no longer has the uncut portion.

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I have no idea what this means.

Attach your *.ipt file and your *.sldprt. example here and end all doubt.

[drunknmunki]

So in this example, let's suppose that I only wanted to turn down the edge by 0.1 mm. I recognize its a bit silly, but there are reasons I might want to do something similar, for example, if I had done all of the cylindrical bits as a revolve. As you can see, there is a giant gap where the rest of the bolt head would be. I don't have access to Solidworks here, but I can assure you that flip side to cut would not remove anything beyond the distance specified in the extrusion.

[SBix26]

In that situation, you are correct, you would need a second profile to define the cut for a specified distance.  Inventor does not have any direct equivalent to the "flip side to cut" option that you describe.

Quickest way is probably, while still in the sketch, hit O (for Offset), quick drag to the outside, type a number ("2" in the example) and Enter.  Now Extrude Cut.  Slightly longer, I guess, but only a problem if you're doing this repeatedly through most of your work.  Then you might have to consider moving back to SW.

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Sam B

Inventor Pro 2022.2 | Windows 10 Home 21H2

[johnsonshiue]

Hi! Or, you can use Delete Face -> Lump Selection -> select the dangling geometry.

Many thanks!

[drunknmunki]

I think the main reason I don't like this is if the number I choose for the offset is too small for a future change. Lets say I pick 2, but then I have to change the OD to 2.5. Sure, its a small issue, but I still don't like it. What can I say, my time with SWx spoiled me.

[paulmWABYD]

Hello, is there an option like "intersect" for the "cut" feature in sheet metal? I've attached a basic part here. Often, I will extrude a part far off into either direction, as I'm not sure how long I'll need it, and then I can draw in my part and cut out the section I want to keep. This works great in SWX, and it's a common practice in surface modeling, as I've seen it. With SWX, the "flip side to cut" and "normal cut" features are all wrapped into the cut extrude feature. As I've drawn this part, I don't think there's a way to create a normal cut and retain the trapezoid shaped part. Can anyone chime in?

[JDMather]

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@paulmWABYD wrote:

... it's a common practice in surface modeling, as I've seen it. 

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@paulmWABYD 

See Attached file.

BTW - it probably would have been best to start a new thread with a link to this thread as reference.

The title of this thread invites controversy.

An alternative to using Surface Modeling would have been to use Unfold then Extrude Intersect - Refold, just like in SolidWorks. (Understanding that this is not quite as simple as Cut Across Bend with Intersection).

A third technique would be Project Flat Pattern and Cut Across Bend...

[paulmWABYD]

JD, thank you for the files. I was looking for a direct sheet metal tool, as I typically make sheet metal parts with surfaces only as a last resort. I prefer to keep all my sheet metal modeling  based on sheet metal tools whenever possible.

The flat pattern projection is interesting, but I'm not sure how I'd use it here. I'd still need to sketch two outer profiles to cut away instead of just drawing the part I want to keep in the middle. Please advise if I've missed something. 

Having intersect functionality in the sheet metal cut tool would be powerful, and it would frequently save a few steps. I'll make a new idea post for it. 

Regarding the post name, as a longtime SW user, I relish a friendly spat.

[JDMather]

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@paulmWABYD wrote:

Having intersect functionality in the sheet metal cut tool would be powerful, and it would frequently save a few steps. 

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@paulmWABYD 
Yep. 👍