Inventor General Discussion

Inventor General Discussion

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Active Member
Bernie38
Posts: 8
Registered: ‎10-29-2011
Message 1 of 12 (399 Views)
Accepted Solution

Selecting Area for Extrusion - Selects more than desired area.

399 Views, 11 Replies
01-29-2014 07:39 AM

Inventor had been working without problems.

I create a sketch with seperate but attached rectangles for solid body modeling.  All constraints and Dimensions are satisfied.  When I try to select the individual areas some select correctly while others combine areas.  Sketch doctor indicates problems but none are visable in the sketch mode.

 

If I create the same sketch without dimensions each area selects as it should with no overlapping.

 

Any ideas?


zxzx5100112855 wrote:
 All constraints and Dimensions are satisfied. 

Not on the file you attached?

I recommend that you make use of obvious symmetry about the origin and pattern features rather than sketch entities.

 

I also noticed that some places you used lines and other places you used rectangles.

In any case, I would wager that the sketch you attached is not what you really really intend. (no symmetry where it appears there should be to me)

And, I would use equal (=) constraints rather than all of those repeated dimensions.

Like I said.... Inventor has trouble with this type of sketch.  Probably the most fool-proof way to build this to delete the short line segments on each end of the center rectangle.  Use the split command to split the lines where the two middle intersect the line going across the ends.

 

It will extrude fine then.  The overlapping lines is what confuses Inventor.

 

Click here for a short video showing how I fixed it.  When you use the split command, you will see a "X" where the break is going to be made.  For some reason that does not show in my video.

 

Kirk

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cbenner
Posts: 3,421
Registered: ‎04-06-2010
Message 2 of 12 (393 Views)

Re: Selecting Area for Extrusion - Selects more than desired area.

01-29-2014 08:13 AM in reply to: Bernie38

Welcome aboard!

 

Post the files here so we can take a look.

ChrisB

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Active Member
Bernie38
Posts: 8
Registered: ‎10-29-2011
Message 3 of 12 (387 Views)

Re: Selecting Area for Extrusion - Selects more than desired area.

01-29-2014 08:37 AM in reply to: cbenner
 
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JDMather
Posts: 28,228
Registered: ‎04-20-2006
Message 4 of 12 (372 Views)

Re: Selecting Area for Extrusion - Selects more than desired area.

01-29-2014 09:24 AM in reply to: Bernie38

zxzx5100112855 wrote:
 All constraints and Dimensions are satisfied. 

Not on the file you attached?

I recommend that you make use of obvious symmetry about the origin and pattern features rather than sketch entities.

 

I also noticed that some places you used lines and other places you used rectangles.

In any case, I would wager that the sketch you attached is not what you really really intend. (no symmetry where it appears there should be to me)

And, I would use equal (=) constraints rather than all of those repeated dimensions.

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karthur1
Posts: 4,329
Registered: ‎04-27-2005
Message 5 of 12 (358 Views)

Re: Selecting Area for Extrusion - Selects more than desired area.

01-29-2014 09:51 AM in reply to: Bernie38

Inventor has trouble with sketches like that.  It tries to figure out the closed profile and it does not always guess correctly.

 

With geometry like that, its better to use rectangles rather than lines.  See my attached file.

 

Kirk

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chad38
Posts: 168
Registered: ‎12-04-2013
Message 6 of 12 (344 Views)

Re: Selecting Area for Extrusion - Selects more than desired area.

01-29-2014 11:00 AM in reply to: Bernie38

I didn't go through and enter all the dimensions to equal each other how you did, especially not the 38mm one. But I drew this up with only lines and none overlapping. And each area can be selected individually without any trouble.

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Curtis_Waguespack
Posts: 3,000
Registered: ‎03-08-2006
Message 7 of 12 (337 Views)

Re: Selecting Area for Extrusion - Selects more than desired area.

01-29-2014 11:12 AM in reply to: Bernie38

Hi zxzx5100112855,

 

IN addtion to the previous hints, note that you can sometimes use sketch points to "break" the sketch into smaller selectable profiles as shown at this link:

http://inthemachine-autodesk.typepad.com/blog/2009/03/no-need-to-trim.html

 

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



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Active Member
Bernie38
Posts: 8
Registered: ‎10-29-2011
Message 8 of 12 (336 Views)

Re: Selecting Area for Extrusion - Selects more than desired area.

01-29-2014 11:16 AM in reply to: JDMather

Thanks for you linput.  Let me reconstruct the part and if I still have problems I will send it to you.TThe original was done using all rectangles but with the error message form sketch doctor I tried to fix what it said was wrong.  The dimensions, least the 38mm were all the same parameter.  Will try equal based off one para,eter (thickness) 

Active Member
Bernie38
Posts: 8
Registered: ‎10-29-2011
Message 9 of 12 (338 Views)

Re: Selecting Area for Extrusion - Selects more than desired area.

01-29-2014 11:17 AM in reply to: chad38
Thanks, I used rectangles
Active Member
Bernie38
Posts: 8
Registered: ‎10-29-2011
Message 10 of 12 (265 Views)

Re: Selecting Area for Extrusion - Selects more than desired area.

01-30-2014 03:46 PM in reply to: JDMather

I started to redo the drawing and check for the ability to extrude each area.  The attached file would extrude on the four outside areas (Created by using a rectangle thend oing an inner offset of the same rectangle, extended the right alnd left side up and down.  Dimensioned sing a created parimeter fjor future mod.  When I added the inner rectangle, dimensined it and when I tred to see if individual sections could be selected for extrusion the center rectangle would select either the section above it as weill as the center or the bottom and the center.  The extrude box does not disply the red cross indicating an error.

 

If I open the sketch doctor it shows Redundalnt points, Missing coincident constraints, overlapping curves, open loops and self-intercecting loops.

The drawing however shows fully constraind on the info bar.

 

I tried doing a project form a "Woodworking for Inventor" video by Steve Widom and every thing came out as it should (Extrusions) but not with what I am doing now.  Any help would be great, thaks in advance. PS tried the "point" approach that was suggested,  Applied points to the four corners but it stillacted the same. (The attached file should no have thises points as there wer deleted using the undo button.)

 

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