Corner blend 2

[looslib]

There has been an active discussion in the PTC Creo community based on the following posting by me last night:

We are trying to model a blend on the corner of a box.
The edges of the box are square, with no blending.
Imagine taking a box and using a belt sander to only radius the corner.
How would you model that in NX?

I don't have access to NX so images only to see what can be done and how easily it can be done in NX.

One of the first replies said to do it in SolidWorks and that was from a long-time Pro/E user. Is SW still Parasolid-based?

If anyone wants to see the PTC community discussion and images:

https://www.ptcusercommunity.com/message/302567?et=watches.email.thread#302567

You may need an account to ptc.com.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[JohnRBaker]

There is no direct way to 'Round-off' a corner, so I had to create a 'spherical' patch and then trim the body. Attached is video showing how this can be done using NX.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[jerry1423]

I think a couple variable blends will work and taper it down to zero at the point that you want it to end

Jerry J.
Milwaukee Electric Tool

http://www.milwaukeetool.com/

 

[JohnRBaker]

Even if that would work, which I'm not sure that it would, it still wouldn't be spherical.

Oh and Ben, I forgot to answer your question, YES, SolidWorks is still using the Parasolid kernel, licensed from us, Siemens PLM Software.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[PintoBeans]

There is no direct way to 'Round-off' a corner, so I had to create a 'spherical' patch and then trim the body. Attached is video showing how this can be done using NX.

John,
After watching the video example you attached, I followed your steps in NX9 and the creation of the "Fill Surface" feature requires that you select "Edges" only. I tried the same thing in NX10 as your example was performed in and the "Fill Surface" Feature now allows you to select curves to create a "Fill Surface". I just wanted to mention this in case someone tries to duplicate your example in NX9.

 

[JohnRBaker]

Yes, that was an 'enhancement' made in NX 10.0 so as to allow the new (and improved) 'Fill Surface' function to more completely replace the now all-but obsolete 'N-Sided' surface.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[PintoBeans]

Thanks for the clarification John, so another words if someone is still using NX9 they could use the N-Sided Surface Feature to achieve a similar surface as shown in your video. I tried this in NX9 using the N-sided surface feature and I was able to create the spherical surface similar to your example. Is there any difference in surface quality between the two features (N-Sided and Fill Surface) ?

 

[JohnRBaker]

Not really, if you use the default options. The new 'Fill Surface', particularly the NX 10.0 manifestation, is much easier to use and can result in a higher quality surface without having to worry about as many options and settings.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[BubbaK]

I doubt that the "Fill Surface" function will give you a spherical shape. Even if it does, you have to construct three circular arcs, first, and this takes some work unless you're lucky enough to have three planar surfaces meeting at right angles.

A more general approach is as follows: suppose you want the corner to be a sphere of radius R.
(1) On each edge coming into the corner, create a tube of radius R
(2) Unite the three tubes. You'll see a point where three edges meet -- this is the point P where the spherical surface should be centered.
(3) Create a sphere of radis R centered at P.
(4) Unite the sphere and the original body.
(5) Do a bunch of Replace Face operations to tidy things up.

 

[JohnRBaker]

Actually, in the example video that I uploaded earlier, the surface created using the 'Fill Surface' function truly was a 'Trimmed Spherical Patch'. Whenever mathematically and topologically feasible, NX will always try to create a 'Canonical' shape. In other words, an exact or primitive shape, that did not require an approximation or application of a tolerance. This holds true for both 3D surfaces and 2D curves. You can try this yourself. Take any spherical, conical or cylindrical body and section it with a Datum Plane and check the type of curves that are created.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[BubbaK]

I tried "Fill Surface" on my skewed plane example, and I got an "alert" saying "some edge cannot have G1 continuity".

 

[BubbaK]

> I tried "Fill Surface" on my skewed plane example, and I got an "alert"
> saying "some edge cannot have G1 continuity".

My mistake. I shouldn't have asked for G1 continuity, because that's not what I wanted. I set all the edge constraints to G0, and I did indeed get a spherical face. NX vindicated. But I'd still be surprised if I got a spherical face when working with anything other than planes. I'll try tomorrow if I have a chance.

 

[JohnRBaker]

I did qualify my statement...

"Whenever mathematically and topologically feasible, NX will always try to create a 'Canonical' shape."

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[BubbaK]

> NX will always try to create a 'canonical' shape.

Well, sometimes it doesn't try very hard. Through Curves or Through Curve Mesh will very rarely (if ever) give a "canonical" surface like a sphere or cone or torus. Have you tried "Fill Surface" with anything other than planes? A sphere-based solution is obviously possible with *any* three surfaces, and it would be interesting to know whether NX bothers to find it.

 

[JohnRBaker]

Some functions, by definition, will only produce a B-surface, such as Surface Thru Curve Mesh and Surface Thru Curves. But Extrudes, Revolves, Fill, etc will, when every thing is just so, give you exact shapes with no approximations.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[NutAce]

Hi John...

A bit off topic, but in your movie I can see some "status bar" showing your history actions. Is this NX10 only or also a setting which can be done in NX9 ?

Ronald van den Broek
Application Specialist
Winterthur Gas & Diesel Ltd
NX8.5.3 / TC9.1.2
HPZ420 Intel(R) Xeon(R) CPU E5-1620 0 @ 3.60GHz, 32 Gb Win7 64B
Nvidea Quadro4000 2048MB DDR5
HP EliteBook 8570W Intel(R) Core(TM) I7-3740QM CPU @ 2.70GHz, 16Gb Win7 64B

 

[JohnRBaker]

What you're seeing is something I added myself using Customize (and yes, it can be done in NX 9.0 as well). I'm utilizing the 'Bottom' Border Bar as a repository for the last 10 'Repeat Last Command' items. I use it as an alternate (and in all honesty, easier to use) version of the 'Repeat Command Drop-Down' found on the upper most Border Bar (where the 'File New', 'File Open', and 'Save' icons are located).

The way you set this up is you first have to have a model where you've performed at least 10 different functions so that the current 'Repeat Command Drop-Down' is full. Then go into 'Customize' and while holding down the 'ctrl' key, drag the icons that you find in the 'Repeat Command Drop-Down', one-at-a-time, starting with the first one and then going in order, from there to the 'Bottom' Border Bar. Once you've copied all 10 icons, leave 'Customize' and remember to save your Role.

Now as you're performing operations, if you wish to repeat any of the last 10, just selection it from the 'Bottom' Border Bar.

Note that you'll have to repeat this for each major application or task that you want to have access to this 'feature', such as Modeling, Drafting, Sheet Metal, etc.

Anyway, have fun ;-)

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[MFDO]

Ben,
If you wish to see how the Cube Corners are done SolidWorks;

[URL unfurl="true"]http://www.solidCADworks.com/temp-files.html[/url] (I uploaded a video to my personal website)




Michael Fernando (CSWE)

http://www.solidCADworks.com

Tool and Die Designer
Siemens NX V9.0 + PDW
SWX 2013 SP3.0 X64
PDMWorks 2013
Logopress3
FastForm Advance
FormatWorks

 

[jpetach]

To make a sharable, file-based, bottom border bar definition that can be centrally deployed from a shared network location, create an ascii text file with an ".abr" extension containing the following:

!
!  Recent Commands NX Bottom Border Bar ribbon file
!
! Place in "%UGII_SITE_DIR%\application\profiles\UG_APP_MODELING" etc. directory.

TITLE  Custom Bottom Border Bar
VERSION 170
ATTACHMENT_TARGET BottomBorderBar
BUTTON UG_TOOLS_REPEAT_LAST_COMMAND_0
!! Uncomment one of the following STYLE directives to adjust the appearance.
!! "DEFAULT" (or no directive) is icon only.
!STYLE DEFAULT
!SYLE TEXTONLY_ALWAYS
STYLE IMAGE_AND_TEXT
!STYLE TEXTONLY_MENU
BUTTON UG_TOOLS_REPEAT_LAST_COMMAND_1
STYLE IMAGE_AND_TEXT
BUTTON UG_TOOLS_REPEAT_LAST_COMMAND_2
STYLE IMAGE_AND_TEXT
BUTTON UG_TOOLS_REPEAT_LAST_COMMAND_3
STYLE IMAGE_AND_TEXT
BUTTON UG_TOOLS_REPEAT_LAST_COMMAND_4
STYLE IMAGE_AND_TEXT
BUTTON UG_TOOLS_REPEAT_LAST_COMMAND_5
STYLE IMAGE_AND_TEXT
BUTTON UG_TOOLS_REPEAT_LAST_COMMAND_6
STYLE IMAGE_AND_TEXT
BUTTON UG_TOOLS_REPEAT_LAST_COMMAND_7
STYLE IMAGE_AND_TEXT
BUTTON UG_TOOLS_REPEAT_LAST_COMMAND_8
STYLE IMAGE_AND_TEXT
BUTTON UG_TOOLS_REPEAT_LAST_COMMAND_9
STYLE IMAGE_AND_TEXT

The ".abr" file (above) needs to be located in the "%UGII_SITE_DIR%\application\profiles\UG_APP_MODELING" directory (or appropriate peer application directory) for each NX application that wants to display the border bar. (See "%UGII_BASE_DIR%\ugii\menus\profiles" for the "application names".)

This displays both the text title and icon for each recent command (as shown in John's AVI). If just icons are desired the 10 lines containing "STYLE IMAGE_AND_TEXT" can be deleted. This is compatible with NX 9 and NX 10.

HTH,
Joe

 

[cowski]

Thanks, Joe!