Offset Geometry

[ToddPig]

I have a sheet metal part that has a few cuts on the faces.  I am trying to create offset geometry, and currently I have to select each line segment by itself, then project this geometry, then create a new line of arc for each segment, then make them equal or colinear, and then I can select the loop and make an offset.

Sorry for constantly comparing Inventor to Solidworks, but its the best reference I have.

In Solidworks, when you project geometry, it turns into sketch geometry (no need to recreate it)  Seecting loops, and tangency in Solidworks also makes the selection process much master.

If somebody has some tips that can speed this process up, it would be much appreciated.

Thanks,

Todd

[JDMather]

I am not familiar with editing image files in Inventor (or in SolidWorks).

[mcgyvr]

When in the offset mode right click and make sure "loop select" is checked..

[Curtis_Waguespack]

Hi ToddPig,

I understand the immediate question, but the fact that I've never really noticed that in a sheet metal part the Project Geometry tool acts differently than expected (by breaking up the project loop between bends), makes me wonder what you're really trying to do here. I suspect there might be a different / better workflow (in Inventor) than projecting that sheet metal edge face ( I could be wrong though).

Can you explain a little bit about what you're intending to do with the offest sketch geometry?

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

[ToddPig]

That works most of the time, the problem is having to recreate the sketch geometry that is used for the offset.

Another example would be, if you have a cube, and then look normal to one surface, and created a sketch on this surface, then click each edge to project the geometry, and then created 4 new lines and made them colinear and equal to the projected lines, then used these new lines for the offset. This is how I currently do it in Inventor and compared to Solidworks, it is very time consuming.

[Curtis_Waguespack]

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@ToddPig wrote:
That works most of the time, the problem is having to recreate the sketch geometry that is used for the offset.

Another example would be, if you have a cube, and then look normal to one surface, and created a sketch on this surface, then click each edge to project the geometry, and then created 4 new lines and made them colinear and equal to the projected lines, then used these new lines for the offset. This is how I currently do it in Inventor and compared to Solidworks, it is very time consuming.

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In that case Project the Face not the 4 edges. But for the sheet metal part I think there is likely still a better way.

[ToddPig]

I am creating a functional gage for in-process inspection. so I need to look normal to the side profile of a sheet metal part (shown), and then create an offset of this geometry that represents the inside of the gage. Another offset (easy to create) represents the outside of the gage.

[JDMather]

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@ToddPig wrote:

Another example would be, if you have a cube, and then look normal to one surface, and created a sketch on this surface, then click each edge to project the geometry, and then created 4 new lines .

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I don't understand why you are doing all of this work. Why not project all 4 lines in one click and then offset all at once?

Can you post an example file?

[ToddPig]

The cube example, was only that, an example, the sheet metal part I am working with is mad of of multiple faces. offsetting the faces seemed to cause lots of duplicated geometry (which is what I'm dealing with now)

[ToddPig]

That is exactly what I looking for, but only know how to do this in Solidworks. Can't figure it out in Inventor (thus my question)

[JDMather]

When you get your part done (the hard way) attach it here and someone will demonstrate the easy way.

[ToddPig]

Here is one of the parts I created in a similar manner.  Very time consuming.

This is a 10/15 minute part in Solidworks, and 45/60 minute part in Inventor.  And at least 100 more mouse clicks.

I have created 3 of these gages so far, and each time, I get a little faster at it, but I know I'm missing something becasue of how fast it cad be done in Solidworks.

[Curtis_Waguespack]

Hi ToddPig,

Try using the Project Cut Edges tool and I think you'll get what you're after. Note that I've not looked at your part just yet, I have things tied up at the moment, but I think this it the tool you're lookiing for.

Project Cut Edges

http://help.autodesk.com/view/INVNTOR/2015/ENU/?guid=GUID-CCDE576C-E260-4762-B2D4-A6492A51F56D

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

[JDMather]

It would be a lot more useful if you also attached the referenced part.

I am pretty sure I would do it differently in Inventor - using a Derived Component.

[ToddPig]

JD, you have had great suggestions in the past, but I think on this one you are getting sidetracked by changing the method. I think that a method change might be a good idea, but I would really like to understand projected geometry and what the value is (compared to projected geometry in Solidworks)

[Curtis_Waguespack · Accepted solution]

Hi ToddPig,

So after looking at your part, I would likely use the Copy Object tool and bring the sheetmetal part into your gage part as a new work solid, and then use the Thicken tool to add the offset. Then model the gage as a seperate solid body and then and use the Combine tool to subtract the work body solid from the gage body.

That workflow relies less on sketches, which is maybe just my preference, but really there was nothing wrong with your method of starting with a projected sketch... the Project Cut Edges tool was really what you were after.

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@ToddPig wrote:

This is a 10/15 minute part in Solidworks, and 45/60 minute part in Inventor.  And at least 100 more mouse clicks.

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It's a 10/15 minute part in Inventor as well, it just takes time with a new set of tools. Hang in there.

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

[ToddPig]

Project Cut Edges was not only exactly what I was looking for, I think it might have been fewer clicks than the Solidworks equivalent.

MANY THANKS!!!!!