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Shape design in NX8
2

Shape design in NX8

RE: Shape design in NX8

Due to the poor image quality, it's hard to make out enough detail on the teeth to give you a decent starting direction.

Are the teeth cross sections all the same similar to a normal gear? Do they twist from OD to ID at all? If they don't twist, create the hollow cylinder and then extrude a triangle on a plane parallel to the cylinder axis to cut out the teeth and then array the extrusion and any blends. If the teeth cross sections twist at all, the extrusion won't work.

Tim Flater
NX Designer
NX 8.0.3.4
Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

RE: Shape design in NX8

(OP)
OK, thanks.
I'll try to send a better picture.
I am more interested in learning the procedure of designing the teeth than in accuracy of the shape....

MZ7DYJ

RE: Shape design in NX8

Here's a starting point - however you may have to do some surfacing rather than a solid. The point being to construct a "cutter" to cut away the shape of the teeth in some manner. This can be accomplished in a simple manner such as this or you can create surfaces and in place of the Subtract (included with the Extrude command) you would use Trim Body, making sure the surfaces extend through the solid completely.

Another approach would be to shorten the length of the Tube and rather than create a cutter, create a positive body to Unite with the top of the Tube to create the teeth.

Be careful adding Edge Blends to Patterns - Unsuppress Edge Blend(5) and watch the Pattern Feature fail miserably. You can get around this by modeling the Tube in a section and model a single tooth (or 2 half teeth) and one of the final steps being rather than use Pattern Feature or Pattern Face, use Instance Geometry.

IMO, the best thing you can do with copying something around in a circular manner if the part proves to be a bit complex - model a "pie section" of the part and use Instance Geometry with a final Unite at the end. This method removes any errors resulting from an Instance or Pattern misinterpreting which Edges to which they are supposed to be applied more often than not. I've had Pattern Face suggested as a workaround, but it too usually fails (with my examples, at least).

You will gain experience and be able to break things like this down quite easily the more you encounter them. I designed wheels for over 10 years and found myself frustrated more than once.

teeth_nx8.prt

Tim Flater
NX Designer
NX 8.0.3.4
Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

RE: Shape design in NX8

Quote (Xwheelguy)

I designed wheels for over 10 years...

So, reinventing the wheel, eh?

www.nxjournaling.com

RE: Shape design in NX8

(OP)
Mr. Backer,
N2 2 seems to be more appropriate.
Thanks

MZ7DYJ

RE: Shape design in NX8

Quote (cowski)

So, reinventing the wheel, eh?

LOL - I wish. The surfaces and using blending tools could be a bear, but the workflows never really changed much.

Tim Flater
NX Designer
NX 8.0.3.4
Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

RE: Shape design in NX8

John,

First off, apologies for changing subjects, but it's somewhat appropriate for this topic.

Any response regarding why the Blend feature gets messed up in the Pattern Feature? This isn't the first time I've ran into Edge Blend not Patterning correctly. Is it working any better in NX8.5 and newer? If not, are there any whispers of shelving or changing Instance Geometry in the future? If there are, I think you have a good case for putting that on hold until Pattern Feature is behaving as expected (if it isn't in NX8.5 or newer versions).

Thanks!

Tim Flater
NX Designer
NX 8.0.3.4
Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

RE: Shape design in NX8

Yes, we've made some changes in NX 9.0 including replacing 'Instance Geometry' with a new 'Pattern Geometry' function using the same tools and interface as 'Pattern Feature'. We've also made it easier to add blends to an existing Feature pattern using the Reference option.

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

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

RE: Shape design in NX8

John,

Thanks for the quick reply. I'm going to make a new thread, as I've got a few more questions related to this.

Tim Flater
NX Designer
NX 8.0.3.4
Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

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