axis not showing up for cylindrical features in part model 1

[lgnx]

Hi,

why axis are not showing up for cylindrical features? i checked with DATUM LAYER, no help. please check the model.

 

[NutAce]

Not exactly sure what you mean. Not showing up? there are no axis present in the file you sent.

When you create a hole or any other cylindrical features, the axis' are not automatically created. If that is what you were expecting.


Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2

Building new PLM environment from Scratch using NX12 / TC11

 

[cowski]

By "axis", do you mean the inferred axis line like in the screenshot below? If so, these are not saved as geometry in the model; it is an inferred, temporary object. I got it to show up for the screenshot by starting the measure command and hovering over the cylindrical face.

www.nxjournaling.com

 

[SDETERS]

May not be 100% on topic, but this is one thing I disliked when moving from I-Deas to NX years ago. I-Deas had an option to display centerlines for cylinders. It would be messy at times, but for simple parts like this it would be a really nice feature. In NX you have to be in a command before you can highlight a face to even view a cenrterline . It was just really nice option in my opinion.

 

[cowski]

The "extract virtual curve" command will create these centerlines for you as associative features or as dumb curves. But you will need to select the cylindrical faces that you want centerlines for, there is not an automatic option.

www.nxjournaling.com

 

[Tingsryd]

@lgnx
I know what you are speaking of; Cowski mentioned is right. The CL should also be visible for things such as infer trim planes when hovering over the cylindrical face.

I looked but could not find a setting for it but I will ask around and let you know if I find it.

NX 12.0.2

 

[Xwheelguy]

Unfortunately in NX Modeling, cylindrical centerlines which appear during certain commands are nothing more than things to reference. Few feature entities other than planes can be derived from the refernce axis without actually creating new curves as described by Cowski. There is NO setting or anything else that will make these reference centerlines visible or more usable than they are already.

If it's something you want added to NX, I strongly suggest filing an ER.

Tim Flater
NX Designer
NX 11.0.1.11 MP8
GM GPDL 11-A.3.4.2
Win7 Enterprise x64 SP1
Intel Core i7 2.5GHz 16GB RAM
4GB NVIDIA Quadro K3100M

 

[multicaduser]

Solidworks also has the option to display virtual center lines, which is needed in order for them to be selectable, or turned off to clean up the display. NX does this dynamically depending on the command, as stated above. Both methods have their benefits and drawbacks.

NX 12.0.1.7 Windows 10

 

[Tingsryd]

@Xwheelguy
I use cylindrical center lines for trimming and splitting solids all the time and without creating curves. For trimming using a cylinder CL I typically pick a CL and a face for a trimming plane which passes through the cylinder CL. The trimmed solid is associative to the cylinder CL and no extra curves are required.

Multicaduser made an excellent point that the CL's only display for relevant functions.

NX 12.0.2
EAP's

 

[lgnx]

Thanks for such huge response.

I understood that,

1. NX doesnt create axis automatically as in Solidworks (which i was expecting).
2. If requird we can create one using 'extract virtual curve' command.​

.


Thank you all.

 

[multicaduser]

Remember NX and Solidworks use the same modeling kernel, what you are referring to is not a geometric issue as much as a display/interface issue. For instance in NX a datum plane can be created between the axis of two cylinders without creating any other geometry. The same thing can be done in Solidworks you just need to turn the display on before creation.

NX 12.0.1.7 Windows 10

 

[Tingsryd]

For some functions it shows up automatically, i.e. to define a plane, but I don't know for what else it will do that. I looked in docs but did not find a definitive answer, sorry.

NX 12.0.2
EAP's

 

[Xwheelguy]

@Tingsryd,

You're correct - you can define a Plane using the reference axes (trimming or otherwise) - that's one of the few things for which they can be used in terms of defining features but I believe it requires additional geometry inputs in order to do so and that's where I was more or less going - singly, they can't be used for much.

As far as OTHER uses, they can be used for Datum feature creation (Datum Planes, Datum Axes - probably not alone but in combination with other entities) as well as many directional or reference direction inputs where a plane or axis might be used; Measure Distance & Angle (at least up to and including NX11 - not sure what if anything might have been botched with the revamped Measure command in NX12); Assembly Constraints will also use reference axes for certain constraint types and that's about all that I'm aware. This is by no means all they can do, I'm sure.

It's just an age-old question that continually comes up with new-ish users. I wish Siemens would have just made them permanently displayed and maybe a bit more robust. The way they are, they seem to cause more confusion than being self-explanatory.

Tim Flater
NX Designer
NX 11.0.1.11 MP8
GM GPDL 11-A.3.4.2
Win7 Enterprise x64 SP1
Intel Core i7 2.5GHz 16GB RAM
4GB NVIDIA Quadro K3100M