Curve selection

[Bishbosh]

NX 5.0.2.2

I have imported DXF curves into a part file that I need to revolve and unite with a model.
Why is it that if I select the revolve icon first then try to select the curves, they are not 'pickable', yet, if I select the curves first and then the icon, I can proceed with no problem.
Extrude function works OK both ways.

Andy

 

[JohnRBaker]

Can you post at least a portion of the model with examples of the curves which behave in this manner?

Also, is it all curves, or just some?

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[Bishbosh]

As requested...

 

[Bishbosh]

Sorry,
Your second question... no just these curves. BTW I did import them as curves and lines with the same result.

Andy

 

[Xwheelguy]

Bishbosh,

Your object filtering in Selection Intent can change when you activate the Revolve command....part of dialog memory I believe.

Check to make sure you have the correct filters set AFTER you've picked the Revolve command. This behavior is consistent (or at least it SHOULD be) through all commands.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

Some people are like slinkies....they don't really have a purpose, but they still bring a smile to your face when you push them down the stairs.

 

[JohnRBaker]

It worked OK for me with NX 5.0.6.1 (which is an internal version of the future maintenance release) however the imported spline is not very smooth. As often is the case, if this profile was imported from a system such as AutoCAD, splines are really created as 'Polylines' which means that it's just a string of small straight line segments collected into a single 'curve'. In NX there is no such thing as a 'polyline' so these 'curves' are converted into splines, however they retain their shape as if they were a series of small line segments.

That being said, you can still create models with them as if they were splines, just that the results will not be as smooth as you might expect them to be.

Anyway, I've attached the model that I was able to create and you should be able to open it in your version of NX 5 although it's possible that it might not update correctly if you attempt to edit it.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[JohnRBaker]

OK, I've gone back to NX 5.0.2.2 and it works just fine. Now when you enter the Revolve command and you're ready to start selecting the curves, make sure that the 'Curve Rule' is set on something like 'Single Curve' or 'Infer Curves', and it should work fine.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[Bishbosh]

John,
That works fine, thank you.

Tim,
I believe there is an issue with the selection filters for Extrude and Revolve commands, Extrude will pick the curves no problem, but I need to set the Curve Rule to Single Curve for the Revolve command.
That's another page in the Tips & Tricks folder for the office!

Andy

 

[Xwheelguy]

Andy,

I've never noticed this behavior, but I may have skipped the version of NX you're running. I did open your part in 5.0.4.2 and it worked just fine with Connected curves.

Connected curves or Tangent curves do not work? Does it select ANYTHING if you use either of these for Curve Rule?

BTW, that's a very ugly spline....71 segments with 70 C0 knots. I'd use IGES next time instead of DXF, if you have the choice, but I think John pointed out what more than likely happened...a polyline.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

Some people are like slinkies....they don't really have a purpose, but they still bring a smile to your face when you push them down the stairs.

 

[hudson888]

DXF has probably rendered that spline down to degree 1. In other words it couldn't deal with the complexity of whatever type of curve it tried to convert. You really want to be using IGES if DXF is going to degrade the curves, assuming that the data wasn't simply created as such in the first place.

Cheers

Hudson

 

[Xwheelguy]

It's a 3 degree spline in NX. It just has 71 segments, with lots of G0 knots.

I haven't worked with ACAD in quite a while, but my best guess is that the spline was originally a polyline due to the way the resulting body looked in the spline section when I revolved the curves in the attached part above (lots of G0 faces; almost faceted looking).

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

Some people are like slinkies....they don't really have a purpose, but they still bring a smile to your face when you push them down the stairs.

 

[hudson888]

Yes sounds like another possibility. You should in that case find more poles than knots, although I suspect that the segments are probably dead straight, and being GO there will be no continuity between segments. The revolved section would be as you described and an Autocad polyline might fit the description of how the geometry was described in the DXF file.

A lot of geometry that may even have been better than that in other CAD systems gets degraded this way when translated using DXF. I think it is because DXF supports fewer complex geometry types and perhaps tends to render a spline to a polyline almost like the series of sraight line moves you'd use for a cutter path, or a faceted model of sorts. Try outputting NX to DXF using some splines and surfaces and then even by re-importing to NX the geometry is degraded.

Cheers

Hudson

 

[Xwheelguy]

I'm going from memory with the number of segments...might have been 70 segments with 71 knots (took a look at it for a few, then deleted it before responding yesterday). Kind of irrelavent really...it was just obscene for a spline, in my opinion.

I've known that DXF can degrade geometry for quite some time now. I avoid it like the plague when it's my project. I'm fairly sure that I read somewhere that DXF will not support splines over 3 degrees....but don't quote me on that.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

Some people are like slinkies....they don't really have a purpose, but they still bring a smile to your face when you push them down the stairs.

 

[Bishbosh]

The profile was created from a Tesascan measuring machine linked to ProComposer software, the output is limited to DXF. The profile is part of a forming operation for deep drawn components and is 'hand finished' hence the irregular profile.
The DXF profile is imported into NX, an undimensioned 10:1 scale drawing is produced which the toolmakers use to manufacture spares (we're in Reverse Engineering land)
The issue was not really with the profile but the selection of the curve (see original post) anyway there is a work-a-round and I thank you for your input.

Andy