chamfer unequal sides? UG-NX4 3

[ravi1982]

my primary aim in modeling a part is to reduce the length of the part navigator (or tree length) as for as possible

Can, chamfer with unequal lengths which are in opposite direction be created, using a singel command (i.e, In the part navigator only one chamfer icon)

for example:-

we have a block which has two unequal chamfer lengths,
say 2mm along the vertical and 1mm along the horizantal direction,

____________________
/ \
/ \
/ \
/ \
/ \
| |
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|_________________________|

( \ => backslash, sorry)

thanks in advance

 

[JohnRBaker]

Yes, that shouldn't be a problem, most of the time. But there are some situations where I've seen where there have been problems with getting Asymmetrical Chamfers to be consistent when applied on more than one edges as part of the same feature, particularly if the edges are not part of a single contiguous loop.

Now there are several reasons why this might happen and we do have people investigating ways to make these situations easier to detect by the software and therefore easier to get right the first time. That being said, we recommend that you try to create the Chamfers as you would like and if you get the results that you were expecting, great. If not, then you may need to create them as separate features. However, if this does happen, we really would like you to contact GTAC and have them open an IR and have you send us your model(s) since we need to try and identify exactly how and why these odd results occurs, but to that end we need more test cases for our people to look at, so as I said, give it a try and if it works, fine. If not do what you need to get the model you desire, but please send us your model(s) so that we have more test cases to examine.

Also, what version of NX are you running and if you are having problems, could you provide a sample part that I could look at?

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
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.

 

[ravi1982]

Thanku John, for answering all my questions

I will try to send a sample part model, as soon as possible,

Me using UG-NX4 japanese language,
One more question is there any option to change the language to English?

 

[JohnRBaker]

The language that NX runs in is usually selected at the time of installation. But I'll see if there is any way to switch it later and get back to you.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
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.

 

[man2007]

John,
How about introducing Flip (or change direction) for each selected edge (loop).

 

[ravi1982]

Hi man2007

Indivisual fliping cannot be done, (i.e, If one edge is fliped then all the other edges selected are fliped automatically)

 

[ravi1982]

man2007 sorry I didnt see john`s name, any how thanks for the suggestion,

 

[tryitagain]

ravi 1982,

to run your ug in different languages, we use a start.bat and add an option for the language.

for the german langugae we use as the option "ge" ...\start_your_nx_.bat de ug and we run it in the english version "en" with ...\start_your_nx.bat en ug

 

[cowski]

my primary aim in modeling a part is to reduce the length of the part navigator (or tree length) as for as possible

While a short model tree sounds like a good goal, you will find it may cause more problems than it is worth. You have already seen a problem with the chamfer command, but it is the problems you don't see that may be worse. For example, if you have a lot of faces you want to taper at the same angle it would make sense to do them all in a single command; but if you later make an edit and only 1 of the faces updates the command is considered successful. In other words, features may fail to update and NX won't issue any warnings (at least this is true in NX2 and earlier, if it has been changed in later versions please let me know). If you taper 1 face in the command and it fails to update on a subsequent edit, NX will let you know. Other commands will behave similarly (eg edge blend, etc).

I'm not advising that each taper and blend need to be applied separately but rather find a balance that works for you (and your coworkers). The shortest feature tree is not necessarily the best feature tree. Experience will show you methods to make your models behave after edits, use those methods to your advantage. If you end up with a short feature tree, great! if not, don't despair - at least you have a robust model.

 

[hudson888]

In the same vein as Cowski above I would go further to say that the aim of reducing the length of the part navigator may seem well intended but is not always good.

To explain a couple of cases in point.

We don't generally like to boolean with feature creation. That is to say we avoid extrude with unite/subtract/intersect. Our reason is simply that during playback it is more maintainable to be able to see the subtraction in the list and look at the extrusion as a separate step on occasion. This isn't necessarily the case all the time, but we do it as a rule because people come to expect to see the boolean in the list and use it to navigate by.

Making the chamfer dialog more complicated where it is not required to so could have the effect of making it harder to use. Just a some users excuse saving an item in the tree when applying blends by selecting several edge sets with different radius values where there is no setback corner or other reason forcing you to make such a complex single feature. From the point of view of anyone later modifying the model finding the 3mm blend becomes quite a bit more difficult.

Please don't just shrink the feature list try to make the model clean straightforward and simple.

Cheers

Hudson

 

[ravi1982]

Yes, I certainly agree with both of you, cawski and hudson888,

Walking in the same steps,
Every part model is different from other, so the methodology by which it is created also differs; my technique in constructing a solid model is as follows
1) First Datum planes, Sketch
2) Create the feature (Extrude, Revolve etc, may use limiting surfaces to avoid boolean or trim)
3) Feature operations (Chamfer, edge blend)
4) Boolean operations (Union, Subtract, Intersection)
5) Feature operation (usually edge blend the most difficult one)

From 1 till 3 the feature is a simple feature, when the Boolean operations are applied to this feature, becomes complex feature (4 and 5).
Generally, reference is taken from datum planes, or else inter link sketch elements using constraint operation, but not from the feature i.e. 2 or 3.

Now, I am facing a problem in the 3rd stage, here I can offered to shrink the feature list (i.e. use a complex feature operation, chamfer or edge blend) because I have not used boolean operation yet.