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Post 1 of 23

Question regarding IV2013 improvements

474 Views, 22 Replies
05-29-2012 05:23 PM

Gentlemen

 

  Can someone please point me to a detailed and complete description of the improvements in the 2013 release, OR

perhaps someone could check/verify that one specific isse has in fact been fixed.

The issue is the conversion of true arcs and circles on a drawing view into splines when the drawing is saved-as an Autocad DWG.

 

A quick test would be is to draw a 2" diameter cylinder, and drill a 1" hole through it's side.

When the drawining view is created with the hole normal to the viewplane, and the drawing is saved-as and AutoCAD DWG, the result of the hole will be ( on 2012 and previous releases ) a continuous spline instead of a true circle.

I have raised this very same question 3 times before, and the last time I was told it will be fixed in rel 2013.

I have the new release in the box, ready to install, but I truly don't want to rush it unless this spline thing is in fact fixed.

 

I would really appreciate it if someone could check it out and reply back with either a yay or nay.

 

Thank You

 

 

 

Post 2 of 23

Re: Question regarding IV2013 improvements

05-29-2012 07:05 PM in reply to: acad-caveman

Short answer...no it has not.  I tried both with AutoCAD Mapping and Visual Fidelity and I got the CV Splines both times.

 

Now after I bring it into AutoCAD, I can convert it to circles in a round about way, but if I was doing this all the time it would probably mean I would make a macro to do it for me, especially if I had a lot of these types of holes.

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Mark Flayler - Senior Application Engineer


IMAGINiT Manufacturing Solutions Blog: http://blogs.rand.com/manufacturing/

Post 3 of 23

Re: Question regarding IV2013 improvements

05-29-2012 07:30 PM in reply to: acad-caveman

Geez Mark, Thank You!

 

Must say I'm quite disappointed but there ain't much I can do about it.

If you don't mind me asking, what is the roundabout way?

I've tried just about every tool I know of in ACAD to no avail.

As it is, I always run Overkill to stich the connecting/collinear entities together, and that tool is awsome.

Unfortunately it does absolutely nothing for splines.

Neither does splineedit.

 

My way - truly roundabout - is to identify all splines, draw a matching circle on a different layer, turn off the layer, delete splines, turn on the layer, trim circles, curse for a while.

Gets exponentially more cumbersome with increased number of splines....

 

Am I really asking for something difficult to fix in Inventor? Is it really unreasonable?

 

Post 4 of 23

Re: Question regarding IV2013 improvements

05-29-2012 07:39 PM in reply to: acad-caveman

I change the PLINECONVERTMODE from 0 to 1

 

This creates arcs rather than linear segments.  Then I convert it with SPLINEDIT to linear arc segments.  That gives me the abiltiy to snap to the center and then the nearest with a new center point circle.  Then, yes I do delete the previous spline.

 

You could write this with a macro to speed it up a little.  You would have an object selection of the spline and then the conversion, the new circle, and then the erase of the selection set (might have to be a temporary group to work in coding).  At least that way the command is executed with little or no typing or input from you and it stops you from having to change layers all the time.

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Mark Flayler - Senior Application Engineer


IMAGINiT Manufacturing Solutions Blog: http://blogs.rand.com/manufacturing/

Post 5 of 23

Re: Question regarding IV2013 improvements

05-30-2012 04:52 AM in reply to: Mark_Flayler

I do a save as to R12 dxf, open the new file, save back to company standard ACAD format (2000  here). The translation turns any splines into arcs & lines.

Mike (not Matt) Rattray

Post 6 of 23

Re: Question regarding IV2013 improvements

05-30-2012 09:54 AM in reply to: mrattray

Hmm....

Is that a 2013 feature?

Just tried it on 2012 and it became a 3D polyline.

 

 

 

Post 7 of 23

Re: Question regarding IV2013 improvements

05-30-2012 10:05 AM in reply to: acad-caveman

Oops, forgot a step. It does work in 2012 (and should work in any edition).

 

1) Save as R12 dxf

2) Open dxf - splines are now plines

3) Explode plines - plines are now lines

4) Save as regular dwg format

Mike (not Matt) Rattray

Post 8 of 23

Re: Question regarding IV2013 improvements

05-30-2012 10:27 AM in reply to: mrattray

I must have something set incorrectly.

I do end up with lines after the explode, but that is what they will stay as even after the DWG save.

 

 

 

Post 9 of 23

Re: Question regarding IV2013 improvements

05-30-2012 10:36 AM in reply to: acad-caveman

That's the point...

Maybe I don't understand what you're trying to accomplish.

The geometery that is the result of the scenario you described above is not true arcs or circles, they are irregular. The way CAD software handles irregular arcs is with splines.

The method I described is what I use to convert flat pattern blanks of complex spline shapes to simple polygonal shapes for our CNC software to be able to read.

What are you trying to do that you need arcs for?

Mike (not Matt) Rattray

Post 10 of 23

Re: Question regarding IV2013 improvements

05-30-2012 11:18 AM in reply to: mrattray

Oh, I got where you've missed my point.

 

Take the example above, a cylinder with a hole through it's side.

The hole is not an irregular shape when viewed from a plane prependicular to the axis of the hole.

It is in fact a true circle, yet Inventor makes it a spline.

 

And since you've brought up the CNC software, that is one perfect example why this is bad.

The above mentioned spline is in fact a circle, which normally is recognized as a drilled feature.

If however it is represented as a spline, I do not know of any software that would recognize it as a drilled hole.

In case of mills/lathes, the result would be a boatload of code for the individual line segments to be profiled.

In case of a punch/laser combo, the hole would be laser cut instead of simply punched.

And that is just the CNC part of the problem.

 

If you want to use the DWG for detailng purposes, you'd never get anything usable to dimension to the hole or radius, even tough that's exactly what they are.

 

 

Post 11 of 23

Re: Question regarding IV2013 improvements

05-30-2012 12:19 PM in reply to: acad-caveman

Ahhhh, I see, I thought you meant the profile of the cylinder edge where the hole's cylinder intersects. And a quick test verifies that you are indeed correct that IV is turning a perectly good circle into a spline.

Unfortunately, I don't know of any way around this offhand. I'll think about it and post back if I have any ideas.

 

Mike (not Matt) Rattray

Post 12 of 23

Re: Question regarding IV2013 improvements

06-11-2012 06:10 PM in reply to: mrattray

I don't see either how you can avoid the splines on a cylinder-cylinder intersection after exporting the IDW to AutoCAD.

A possible (although painful) remedy is to use the FLATTEN command from the AutoCAD bonus tools to convert splines back to arcs (but you will probably get a lot of arcs instead of the expected single circle).

 

Bob




Bob Van der Donck


Principal UX designer DMG group
Post 13 of 23

Re: Question regarding IV2013 improvements

06-11-2012 10:23 PM in reply to: bobvdd

Please note that IT IS NOT !!! a cylinder-cylinder intersection!!!

It is a view from a plane that is normal to the axis of the through hole.

Regardless of what solid body the hole goes through - cylinder, angled surface or any other irregular nonplanar surface, it is a hole.

IOW If I created it as a hole feature or a circular cut from a plane, it should always be a full circle when viewed from the same plane, no matter what.

 

This problem has existed in Inventor 2010, 2011, 2012 and now in 2013 as well. It was incorrect in 2010 and it remains to be incorrect in 2013. I cannot think of any reasonable explanation for this to be so.

 

Post 14 of 23

Re: Question regarding IV2013 improvements

06-12-2012 05:24 AM in reply to: acad-caveman

Well I don't see it as inexplicable, it makes sense if you think about it from a program's point of view. Even though in the 2D world that shape is a true circle, in the 3D world that edge is not. As we know IV looks to the 3D model for all of it's information, so it's not surprising to me that it would translate that geometery to a spline. Incorrect, but not inexplicable.

 

I made this to test a theory I had for you. It didn't work but the image might save you some typing explaining the problem.

Mike (not Matt) Rattray

Post 15 of 23

Re: Question regarding IV2013 improvements

06-12-2012 08:35 AM in reply to: mrattray

I don't expect we will change this behavior anytime soon.

 

If it holds you back in your AutoCAD work, what I would suggest is to work with a drawing sketch that is "associated" to the view (= select the view first and then use the "Create sketch" command)  and project all geometry from the view into that sketch and then use this sketch block in AutoCAD to do your CNC work.

 

It looks like the projection operation restores the circles or arcs as long as your view direction is parallel to the hole direction.

 

Bob




Bob Van der Donck


Principal UX designer DMG group
Post 16 of 23

Re: Question regarding IV2013 improvements

06-12-2012 09:32 AM in reply to: bobvdd

This might give a better understanding of how Inventor displays your model in a IDW. The first capture I used my SpacePilot to rotate the drawing 90 The large verticle line to the very left is the drawing sheet. The second capture is the normal view.

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Post 17 of 23

Re: Question regarding IV2013 improvements

06-12-2012 09:36 AM in reply to: mrattray

With the risk of sounding like an absolute jerk, that is quite disappointing. Specially the fact that you've called it

a "behavior" instead of a "mis-behavior".

This, coming from the company that is arguably one of the strongest pillars of the CAD industry, is truly disappointing.

 

Really, I should project edges in Inventor (Adesk) and export them into AutoCAD (Adesk) to get usable geometry?

Is that really the best that Autodesk can and will do?

 

Believe it or not, I do have another workaround as well.

I can take my Inventor solid and export it as STEP. I then take the STEP file in Solidworks 2007, create the drawing views, save them as DWG and use that in my further work.

Would you recommend that Inventor subscription cutomers go out and purchase a copy of Solidworks if they want their solid models transferred properly into an AutoCAD DWG?

 

 

mrattray:

 

Thank you for your replies. In response to your theory, please look at the attached drawing.

You'll see that the cylinder-cylinder transition of the two extrusions produce a true line when viewed from a normal plane, yet the very same view produces a spline for the hole.

Note that neither of those entities are actually intersecting the plane, but are at a varyiung distance from it, yet the line comes out correct, while the hole does not.

 

 

 

 

Post 18 of 23

Re: Question regarding IV2013 improvements

06-18-2012 01:36 PM in reply to: mrattray

"""

If it holds you back in your AutoCAD work, what I would suggest is to work with a drawing sketch that is "associated" to the view (= select the view first and then use the "Create sketch" command)  and project all geometry from the view into that sketch and then use this sketch block in AutoCAD to do your CNC work.

 

It looks like the projection operation restores the circles or arcs as long as your view direction is parallel to the hole direction.

"""

 

 

  Ok, there must be something I'm missing.

I've tried just about everything, and no matter what, none of the projected edges show up in AutoCAD.

I can draw a circle in the sketch and it will transfer just fine, but projected edges do not.

I can "trace" the projected linear edges by drawing lines from endpoints to endpoints and they will show, but I cannot "trace" the projected circle because it is apparently a spline in Inventor DWG as well. IOW if I want to create a circle to overlay the projected edge, I cannot snap to it's center point because it does not have one.

 

Can someone please suggest what I might be doing wrong???

 

 

Thank You

 

 

Post 19 of 23

Re: Question regarding IV2013 improvements

06-18-2012 01:49 PM in reply to: acad-caveman

Use "Break link" command on the projected edges and remove the "Sketch only" property from those projected edges.

You will of course also have to make the edges in the drawing view invisible to avoid displaying duplicates.

 

Bob




Bob Van der Donck


Principal UX designer DMG group
Post 20 of 23

Re: Question regarding IV2013 improvements

06-18-2012 02:45 PM in reply to: mrattray

Bob Thank You, that worked .... to show the projected edges that is.

Unfortunately the projected edge in the sketch is still a spline.

As soon as the link is broken, the control points of the spline become visible and ... well it isn't a circle any more, not even in Inventor.

 

 

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