"Convert Entities" in Inventor

[Anonymous]

Hi All,

I Have searched and simply can't find the answer to this basic question-

How do you "Convert Entities" (Solidworks), "Copy Geometry" (Creo) in Inventor? I've tried the Project Geometry tool, but it only brings in reference geometry. The geometry I am projecting is rather complicated and I don't want to have to recreate in every sketch and part.

What am I not doing or is there some other approach to this situation?

BTW- The geometry I am trying to reference in my various parts is Derived from a common Skeleton part file made up of 2D Sketches and planes.

I thank you in advance.

Jeff

[Curtis_Waguespack]

Hi AutoMCD,

If I understand correctly, you can use the Derive tool:

http://help.autodesk.com/view/INVNTOR/2014/ENU/?guid=GUID-0A5D9D9B-8B6E-48A2-A1D9-54C0A57D171B

and/or the Copy Object tool:

http://help.autodesk.com/view/INVNTOR/2014/ENU/?guid=GUID-73E87DDB-2D73-45CA-958F-1B5019AC7A27

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[Anonymous]

Hi Curtis,
No that's not it. Geometry is already successfully Derived to my other parts. The trouble is in converting derived geometry into usable sketch geometry in the new part(s)- without remaking it.
Jeff

[Cadmanto]

Jeff,

Not sure exactly what you are saying in regards to project geometry only bringing in reference geometry.

In Solidworks with the convert entities you get something like this.  Which can be used to create features from.

Thus in Inventor with the project geometry command you can do the same thing.

As long as it is enclosed like any other sketched lines, arcs and circles it will project into regular features.

Can you either post your file or at least show some images?

If this solved your issue please mark this posting "Accept as Solution".

Or if you like something that was said and it was helpful, Kudos are appreciated. Thanks!!!! 

     

[JDMather]

Attach example  files here (SolidWorks or Creo will do, if you don't have Inventor example).

Some one will show you the equivalent technique in Inventor.

[Anonymous]

Here is file I am referring to. It has my derived "skeleton" file in it. I make a product that has 4+ parts in it, each using the skeleton's geometry and planes (a ring that I resize). Typically I would now "project geometry" from skeleton onto a plane and extrude, cut, chamfer etc... for a part. Then do same for the other parts that fit to it in an assembly.

Let me know if this is unclear.

Thanks,

Jeff

[JDMather]

I do not see a plane or part face to project on to?

I do not see any geometry to cut?

Did you intend to attach another file?

I have SolidWorks, can you attach your SolidWorks example here?

Did you intend to attach an assembly here?

Are you familiar with Inventor Derived Components (works a bit differently in Inventor)?

[Cadmanto]

I get this error when trying to open the file in 2014.

What version is the file created in?  Weird that I can view it.

I even tried opening it up in Solidworks and it just freezes trying to process.

If this solved your issue please mark this posting "Accept as Solution".

Or if you like something that was said and it was helpful, Kudos are appreciated. Thanks!!!! 

     

[JDMather]

---

@Cadmanto wrote:

  Weird that I can view it.    

---

View what?  The bitmap Thumbnail preview?

iProperties indicates R2015 SP0

Anything could be used for the Preview Picture

[Cadmanto]

Yes, the bitmap preview in windows explorer.

That would explain a lot why I can't open it.  I didn't think to look at the properties, because my experience has been when it is a newer version it indicates that in the error message.  I have no idea what the error message I posted and am getting means.  Do you have 2015?  I have it, just not loaded.

If this solved your issue please mark this posting "Accept as Solution".

Or if you like something that was said and it was helpful, Kudos are appreciated. Thanks!!!! 

     

[JDMather]

Yes, can only see the iProperties in latest release.

[Anonymous]

Here are 2 Solidworks jpegs- extrusion process from sketch where geometry came from derived skeleton file. And, the assembly I eventually make with the assorted parts that share this skeleton file.

Also, I changed Inventor file to reflect Projected geometry necessary for this particular part. It is in "Body" sketch. Typically I would now start trimming away parts of projected geometry to create the extrudable sketch.

Thanks for your help trying to figure this out everyone.

Jeff

[Anonymous]

Yes, Inventor 2015. Just downloaded it.

[Anonymous]

Ah, very sorry. I forgot the all important skeleton file- necessary to open B1.ipt file.

Jeff

[JDMather]

You can get screen captures far more easily by either of these two techniques

1. Hit Print Screen upper right corner of keyboard and then Ctrl V in MS Paint

or

2. Go to the Windows Globe in lower left corner of the screen and type Snipping and use the Windows Snipping tool.

I can't see your SWx browser.

In any case, I am not familiar with using either SolidWorks or Inventor as an image editor - I was expecting *.sldprt and *.sldasm files.

You can use one of three techniques -

1. Multi-body solids - the same as in SolidWorks

2. Derived Components - works a little differently than SolidWorks

3. Top-down in-context assembly modeling - the same as in SolidWorks.

Once you have attached your SWx files here - I can demonstrate all three master (skeletal) modeling techniques in Inventor.

[Cadmanto]

Jeff,

Not sure what I am missing, but I am able to take your skeleton model and create geometry using the project geometry.

If this solved your issue please mark this posting "Accept as Solution".

Or if you like something that was said and it was helpful, Kudos are appreciated. Thanks!!!! 

     

[Anonymous]

Cadmanto and everyone, thanks for trying with me on this one (wish we could be in the same room for 5 minutes and I suspect we'd solve this one quickly).

Instead of my particular case, let me ask instead- how would you do the following?

1. Make a circle with bisecting line on XY plane in a sketch and "finish sketch"
2. Make a new sketch and project that same circle and line onto same XY plane.
3. Trim circle in half at bisecting line.

My problem is- how do I have trimmable geometry from projected geometry? When I do example above the only modification functions that allow me to select geometry are "offset" and "mirror". What am I not doing right?

Jeff

[JDMather]

Projected geometry is projected geometry - you don't trim it.

In general - trimming isn't needed as Inventor will let you select enclosed contours.

If you really want to trim it - RMB Break Link to the original or convert to Construction and sketch overtop the portion you need.

[CCarreiras]

Hi!

Project the geometry and break the link.

You will have to apply some constrains to fully constrain the sketch.

Did you find this reply helpful ? If so, use the    Accept as Solution or Kudos - Thank you!

[Cadmanto]

Jeff,

I would imagine you would be correct that you could get an answer quickly if we were all in a room together.

JD is correct the the project geometry cannot be trimmed.  I can't remember if convert entities could be, but that might have been the root question to be asked in the beginning.  But like most threads, where they go often looks much different then where they end up.

Best of luck and hope you find the solution that works for you.

If this solved your issue please mark this posting "Accept as Solution".

Or if you like something that was said and it was helpful, Kudos are appreciated. Thanks!!!!