How to present gear teeth in NX 2D-draft

[SimoSakkinen]

Hello All!

I have frequently ended up reading through threads at eng-tips -forums as result of searching answers for engineering-related topics. Now it is time for my first post. I work as a designer at mechanical power transmission industry and have previously been using SolidEdge as 3D-CAD. Presently I have changed to NX10 and of course, facing many many modeling- and drafting related differences.

It would be extremely interesting to hear from techniques regarding how to efficiently present gear teeth in NX 2D-drawings that are based on 3D-models. As I have been trying different methods, the most feasible I have currently come up with (illustration attached) is to generate sheet bodies in 3D-model which present root- and reference diameters. These sheet bodies are set on different layers, so they can be called visible if necessary (in suitable 2D-section view or assembly section). After setting this layer visible, one can set correct cross-hatch in section view.

In most common cases in manufacturing documents, it is not necessary to present gear teeth in 3D-model. However there are exceptions, such as the gear in illustration that includes internal teeth of a release coupling. I should be able to present the shape of the chamfer at tooth end in manufacturing drawing. Now as it can be seen in the attachment, this exact tooth presentation in 2D-section view looks quite messed up and should be cleaned in order to produce a clear drawing. In addition actual tooth geometry can lead to incorrect diameter values as the section plane can cut teeth in arbitrary plane (not necessarily from tip-to-tip).

Now the most interesting question is: How to efficiently "simplify" gear teeth in 2D-views (basically remove the teeth cut feature at defined views)? In SolidEdge there were a "Simplify part" option in 3D-modeling environment where one can for example suppress features which are not wanted to be shown in simplified model. In 2D-drafting environment it could be selected in each view whether or not to show detailed or simplified model. This feature was very convenient while modeling gears.

Thank You for Your comments!

Best Regards,
Simo

 

[NutAce]

Up to NX 5 there was the function "Simplify Body" (which can still be activated by the way with dedicated variable).
For single parts, not in an assembly,currently I would just create an associative copy of the body using "Extract Geometry". From that Body you can easily remove unnecessary features with Synchronous modeling techniques.
The copy you can of course place on another layer..

Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2
HPZ420 Intel(R) Xeon(R) CPU E5-1620 0 @ 3.60GHz, 32 Gb Win7 64B
Nvidea Quadro4000 2048MB DDR5

HP Zbook15
Intel(R) Core(TM) i7-4800MQ
CPU @ 2.70 GHz Win7 64b
Nvidia K1100M 2048 MB DDR5

 

[SimoSakkinen]

Thank You for reply!

That is a good tip and is one possible method to perform exactly what I need.

Unfortunately it seems that extract geometry loses the information of features (which is no surprise as it only copies the body geometry). The resulting problem is the manual selection of all tooth faces, which in case of let's say for gear with 100 teeth is quite a job. If the features were still active in the extracted geometry, one could only select the tooth cut and its circular pattern, and maintain associativity between original tooth feature and simplified geometry.

Anyway, that geometry extraction is feasible solution to start with! And in addition, maybe this method is quite efficient if correct selection method is used when deleting tooth faces.

Best Regards,
Simo

 

[NutAce]

When you make use of the Face Rule selector it will make it a bit easier for you..
With the correct selection it will automatically select all faces connected to the face you select.

Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2
HPZ420 Intel(R) Xeon(R) CPU E5-1620 0 @ 3.60GHz, 32 Gb Win7 64B
Nvidea Quadro4000 2048MB DDR5

HP Zbook15
Intel(R) Core(TM) i7-4800MQ
CPU @ 2.70 GHz Win7 64b
Nvidia K1100M 2048 MB DDR5

 

[SimoSakkinen]

That indeed makes it easier to select all faces of a tooth gap, good tip!

I came up with another improvement: It could be wiser to have the "simplified" revolved form with all details first finished, and at this point use "Extract geometry" and cut the tooth 3D-geometry in the extracted body in different layer. This way the dimensioning in 2D-drawing can be done reliably with the simplified model, and if necessary the extra layer with exact tooth geometry can be called visible in certain drawing views or at higher assembly level. Also this method does not require manual selection of tooth gaps.

Best Regards,
Simo