Drafting: define a view 1

[cowski]

In drafting, is there a way to take an arbitrary view of the part and define it as the 'front' view then generate a trimetric view from that?

I seem to remember reading about some feature like this in either the NX5 or 6 marketing literature, but cannot find anything in the help files. I am currently running NX6.

 

[JohnRBaker]

This is another example of why we recommend that you work in a Master Model mode where the Drawing is an Assembly and the model being drafted is a Component. If you do this you can then physically rotate, using...

Assemblies -> Component -> Move Component...

...the 'Component' around in the Drawing Assembly (but you must have toggled OFF the display of the Drawing sheet first) until you have oriented the Component relative to the DRAWING Assembly's Absolute CSYS in the manner in which you wish it to be. Generally speaking, if there is some specific 'feature' on the model which you wish to be shown in what we used to call 'true view' back in my drafting board days, your best bet would be use the Reposition option as this will allow you to align X-Y references in your model with the X-Y references of the Absolute CSYS of the Drawing Assembly.

Anyway, give it try and see if this provides you with what you need.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
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.

 

[cowski]

Thanks for the reply. I do use the master model approach, and the process you describe is what I have been using. It works well for single parts, but I was hoping there was an alternative (especially for assemblies).

Is there a way to make your own 'canned views' as described in the first post (or maybe that was just for modeling)?

 

[JohnRBaker]

There's no reason that you can't treat an Assembly as if it were a single Component, which when working in the Master Model mode, it is (simply think of your Assembly as a Sub-Assembly when in the Drawing file).

As for creating a set of user defined views which you can use instead of the default views, while it's possible, the system will still consider the Absolute X-Y plane as being the default 'Top View' orientation no matter what and therefore all of the other 'canned' views will key off of it.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
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.

 

[SDETERS]

Will this be a feature added in NX7.5 drafting(Be able to define your front view). At the current time in I-Deas we can create a front view of a part no matter of the orientation or where the part was modeled at.

 

[JohnRBaker]

No, there were NO changes made in this area as there was NO NEED TO since we already provide for this as I've described above. Besides, there is nothing stopping you from creating any number of User Defined Views anytime you wish in your detail Part file and these views can be used, even when working in the Master Model mode, when adding views to your Drawing.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
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.

 

[SDETERS]

That makes sense now that I thought about it a bit. What is the drafting package you mentioned that is coming out with NX7.5 that will be no extra cost to I-Deas users. Sorry I did forget the name. Is there any literature on this yet of the functions of this pacakge? Thanks

 

[hudson888]

I don't know why anyone needs to have standardised canned views any more anyway. Sure they'll always exist, but whenever I want to set up to an orientation that is not aligned to the axes of the absolute coordinate system I just set up my WCS to the face that I want to look at snap the view to that orientation and then save the view under View>Operation>Save As and give it a name. I can then go into drafting and just add that view as a base view to the sheet and cast projected view straight off that one.

Now I expect that is a little more trouble than having everything always done automatically for you by your templates, but compared to moving the model off absolute in order to align it to the canned views, then IMHO the effort is about the same.

I'd add that I usually work to a project absolute co-ordinate system meaning that static parts often don't need to be mated in assemblies. For larger projects such as automotive design this has always made sense. So I would use the above described method most of the time, and I have never suffered any difficulties as a result.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[JohnRBaker]

Originally the 'enhanced' NX Drafting package was being called 'NX Drafting Plus', but recently it appears that the name has been changed to 'NX Power Drafting'. Now it could change again before it's finally released (with NX 7.5, which is currently scheduled for Spring, 2010). As for when more detailed information will be available, that will not be until we get closer to the official 'launch' of NX 7.5, which will not be for at least 2 or 3 months yet.

However, you should keep tabs on our website...

http://www.plm.automation.siemens.com/en_us/

...since as soon as there is anything to be said about this and other aspects of the NX 7.5 release, this is where you will see this information first.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
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.

 

[cowski]

I can then go into drafting and just add that view as a base view to the sheet and cast projected view straight off that one.

NX makes the projected views quite easy, but does anyone have any tips or tricks for generating an isometric or trimetric view from your saved view?

 

[cowski]

I guess what I'm after is once I have a front view, how much do I rotate that view to end up with an isometric or trimetric view. A google search is providing hints for isometric case but not much information for the trimetric case.

 

[cowski]

I got the answer for the isometric case from wikipedia.

when taking a cube, this is done by first looking straight towards one face. Next the cube is rotated ±45° about the vertical axis, followed by a rotation of approximately ±35.264° (precisely arcsin(tan 30°) ) about the horizontal axis.

http://en.wikipedia.org/wiki/Isometric_projection

Still looking for the trimetric view.

 

[JohnRBaker]

For a Trimetric view, follow the same steps only use -51.57° and 22.91° respectively.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
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.

 

[cowski]

Thanks John.

 

[hudson888]

Cowski,

I know that you're no slouch so you must want to do this for some kind of reason. So humour me and riddle me this... What's so useful about a technically isometric view as opposed to something that looks near enough. I just don't have that much use for them besides illustrative purposes?

Like many people I usually add a view in the top right hand corner of my drawing sheet just to show what the part looks like. It is just for illustration purposes. So I simply add a base view and then use the orient view tool to manually rotate the part into a position that shows enough of the part to illustrate what it looks like. I have never been able to set up a template file that successfully guesses this for me so I'm as happy to spend a couple of seconds doing it myself.


Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[JohnRBaker]

Well in some industries there are standards when it comes to so-called 'illustrative' views included on a Drawing, such as the Auto industry which uses something called 'Dimetric' views, which consists of 16 predefined view orientations conforming to an old drawing office standard which is still in use today. NX supports the automatic creation of these 16 additional 'standard' views, but out-of-the-box, this feature is turned OFF, however it can be toggled ON in Customer Defaults.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
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.

 

[hudson888]

John,

Agreed! But then the GM system to which I gather you refer relies upon actually modelling in Car Line (Absolute), as I referred to earlier.

If we're talking about fasteners or the odd generic part then I don't know that it matters. I guess that anything else modelled close to absolute and then mated into an installed orientation that was required to be reflected in a drawing view probably needs to be copied from the assembly and pasted to the master model method drawing assembly in order to maintain the correct spatial attitude. I didn't think that was what Cowski was getting at but if it does matter to some users then I don't think we explored that option before.

For the record in automotive work the likelihood is that unless the part is first used elsewhere the preference or requirement will be to move the geometry inside the component part file to the installed location relative the Car Line absolute so-ordinate system.

Anyway I hope that offers some insight as to your options.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[JohnRBaker]

Hudson, I agree with you nearly 100%. After all, I'm an old machine designer (did it for over 14 years) and each part was drawn/modeled as much for how it would look when the detail drawings were finally made as they were for how they fitted in with the rest of the machinery. Besides, we constantly reused existing and off-the-shelf parts so virtually nothing was ever modeled 'in place' as it were (with the possible exception being machine guards and ductwork).

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
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.

 

[cowski]

I should have started my first post with my problem and goal rather than asking whether a certain feature existed in NX. My 2nd post confused the matter for which I apologize.

My question has technically been answered, but I'll give a little background to hopefully clear things up. The company I work for makes small consumer goods and 90%+ of the parts are unique to each model, so we create them in 3D space 'where they belong' which avoids much hassle with assembly constraints. We use master model for our drawings which generally have a front, right, top, and a trimetric view of the part. The trimetric view serves as a pictoral view of the part, but we also use it to call out surface finish and textures for the cosmetic surfaces. I will reorient the part to get the important features in the dimension views, occasionally either the front view that I want for dimensioning will not lead to the trimetric view that gives the most information or the part will require callouts on the front and back so I will use multiple trimetric views. I have been rotating it to something close in modeling, saving the view, and adding it to the drawing. I was hoping there was a way to snap to a 'new front view' and generate a trimetric view off of that. I don't work to a drafting standard that has well defined definitions for pictoral views, I was just hoping to speed up drawing creation a little bit and make the views look more consistent.

On my journey of discovery with Wikipedia, I got a good refresher on axonometric views. If you rotate the model such that all 3 axes (X, Y, Z) are foreshortened equally, you end up with an isometric (same measure) view. When 2 of the axes have the same measure it is a dimetric view, and when the 3 axes have different measures it is a trimetric view. There is a well defined set of rotations to get an isometric view, but there is an infinite number of possibilities for a trimetric view. I had mistakenly thought that a trimetric view was a certain (but different) set of rotations than an isometric view. Another thanks to John for telling us the rotations that NX uses in its definition.

 

[hudson888]

Cowki,

Now that you've read up on it and understood all of the possibilities. I have created something for you that if you import it into your drawing templates will furnish them with all the extra views that you could probably ever want. Make sure to tick on the Import Views and Cameras option and you should be good to go.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum