Use edge in a sketch

[Anonymous]

Can I "use and edge" in a sketch?  It is a solidworks command that is very helpful.

If I am sketching something and I want it to match some existing geometry, I project the reference into my sketch.

If I want to draw a line, arc, circle, spline or anything, I have to fully re-create it.  Is there a way to tell IV to just use that edge, no matter what it is to create geometry?

Any suggestions?

[johnsonshiue]

Hi Ronald,

In Inventor, you will need to project or include sketch. In 2D Sketch, you need to use Project Geometry command. In 3D Sketch, you need to use Include Geometry. In general, Inventor sketch only deals with sketch geometry. It does not work with other type of geometry.

Many thanks!

[mcgyvr]

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@Anonymous wrote:

If I want to draw a line, arc, circle, spline or anything, I have to fully re-create it.  Is there a way to tell IV to just use that edge, no matter what it is to create geometry?

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Can you show an example where you need to re-create?

Normally..If you project geometry from another feature you can use that without re-creating it to create additional features from it..

[JDMather]

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@Anonymous wrote:

Any suggestions? 

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I assume that you are familiar with Convert Entities in SolidWorks.

The equivalent in Inventor is Project Geometry.

There is a way to set up Inventor to auto-project such that it sort of acts like SolidWorks, but it will more likely cause more frustration than simply manually projecting your edges.

I recommend that you attach an example file here to get suggestions on an efficient Inventor technique.

[Anonymous]

@JDMather Yes, I am sorry, I did mean the SW function convert entities.

When I use that in SW, it creates a line (or arc or spline...) that is geometry.  When I project geometry in IV, all it does is create a reference I can use to dimension to.  How do I use the projected geometry as geometry and not just a reference. 

[JDMather]

Attach your example file here.

[Anonymous]

In SW, I created a block and then a sketch:

Next, I convert one edge of the block to geometry:

Now that converted entity is a full blow line in the sketch:

When I project in IV:

All I get is a reference.  If I want that to be geometry, I have to create it.  It is easy with a line, but with complex geometry, it takes time.

  

I hope that makes more sense.

[JDMather]

Oh, man - your going to make me read and decipher pretty pictures.

This would be so much easier with the *.sldprt file.

Back in a bit with my description of Inventor technique.

[JDMather]

Why are you manually creating this line?

The Project Geometry works the same as Convert Entities.

Pick an edge - it project the edge.  Pick a face - it projects all edges of the face.  No difference!

[mcgyvr · Accepted solution]

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@Anonymous wrote:

In SW, I created a block and then a sketch:

Next, I convert one edge of the block to geometry:

Now that converted entity is a full blow line in the sketch:

When I project in IV:

All I get is a reference.  If I want that to be geometry, I have to create it.  It is easy with a line, but with complex geometry, it takes time.

I hope that makes more sense.

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Works the same in Inventor.. 

[Anonymous]

UUUUGGGGHHHHHH

Mind blown.  I had no idea all I needed to do was use projected geometry.  The lines never change color - I did not think they were anything but references.  I have been killing myself drawing lines I did not need to draw.

Pass me the dunce cap.

Thanks for your help and patience.

[mcgyvr]

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@Anonymous wrote:

UUUUGGGGHHHHHH

Mind blown.  I had no idea all I needed to do was use projected geometry.  The lines never change color - I did not think they were anything but references.  I have been killing myself drawing lines I did not need to draw.

Pass me the dunce cap.

Thanks for your help and patience.

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The lines do change color when projected..

Or they should..

However.. maybe you just have autoproject turned on by default.. That may explain what you just wrote..

Do you have .."Autoproject edges for sketch creation and edit" checked in .tools..application options....sketch tab?

[Anonymous]

I guess what I meant was, the projected edges turn yellow and stay that way.

Geometry is some sort of green and when it is contained, it turns some sort of blue.  Since the projected lines just stayed yellow, I figured they were only good for constraining and dimension-ing.

The option you suggested is not selected.

[JDMather]

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@Anonymous wrote:

... yellow 

... green

... blue. 

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Yes, all of these color codes are simply Inventor's way of letting you know where/how the geometry originated and it's current state.

Just watch out for pink (magenta) lines as this indicates "sick" geometry.

Not just Blue/Black/(Grey) like SWx (although you can set up SolidWorks options to give you similar color indications) 

It is construction-only line if it is dashed (similar to SolidWorks centerline/construction).

[Anonymous]

That is what got me.  The dashed line thing is good to keep in mind.  The projected geometry is different enough (even if it is only colors) from what I am used to that I get turned around.

Thanks.

[Anonymous]

Of course once I think I am out of the woods, I figure out something that does not work.

I created a video showing a situation where the projected geometry cannot be used to form a profile.

At the start of the video, I have all the projected geometry on the sketch and have drawn a single line.  Then I create a revolve.  When I try to pick the profile, all I can get is the tip.

When I create lines and arc's, using nothing but the projected geometry as reference, the profile creates fine.  You can see that later in the video.  Any idea why that would be or what could be done about it?

I would love an IV work around...

Thanks.

[SBix26]

Can you include the video in your post?  Or, even better, the file?

Without the video or the actual file, I can't tell what happened in yours. In general, the reason why a region isn't selectable is that it doesn't connect all the way around.  If your profile has elements added that cross over but do not intersect with the projected elements, there will not be a valid profile.  That is, if there is not a point (e.g. end of line, center of arc, etc.) the profile finder can't "turn the corner".  The solution is either to add a sketch point that is constrained to both elements, or trim/extend one or both.  It's not to difficult to figure out these profile issues once you understand that there must be a point constrained to both elements in order for Inventor to see them as connected.  In your example further up, you trimmed your circle to the edge line, which constrained the arc's end points to the line.

Hope this helps,

Sam B

Inventor Professional 2018.2.3
Windows 7 SP1

[Anonymous]

I thought i did include the video, sorry - I think i got it this time 🙂

[TheCADWhisperer]

Can you Attach this simple file here?

It looks like some projected edges should be turned into Construction.

Crossing window select geometry that is not involved in the Revolve, right click and select Construction.

[Anonymous]

Take a look.  It is revolve 4.  I had to strip away some features, so it looks a little foolish.

Thanks.