NX5 - Untrim VS Enlarge 1

[ewh]

What are the benefits of Insert->Trim->Untrim compared to Enlarge surface?
It seems to me to actually give you less control over the resulting surface, and I am curious as to when Untrim be preferred.
Thanks!

Believe it if you need it or leave it if you dare. - [small]Robert Hunter[/small]

 

[cowski]

The only time I can remember using untrim was with imported geometry (mostly IGES files). Sometimes when there are gaps and mismatched edges you can untrim a few surfaces and retrim them. Doesn't work 100% of the time, but it is a good first attempt.

I suppose enlarge could also be used in this instance, but if the underlying surface geometry is there, it seems like a better idea to use it rather than extrapolate a surface with the enlarge command.

 

[Xwheelguy]

I think that we're talking about 2 different commands here and both are using the exact same icon yet performing slightly different operations.

One command is found under Edit Surface -> Sheet Boundary -> Remove Trim. This command will untrim a trimmed surface back to its original shape or area. Remove Trim will ONLY work on surfaces that are not Sewn to another body, unless you first Extract the surface you want untrimmed. Most users are probably familiar with this one if they have been working with imported surfaces that will not sew together and need to be untrimmed and retrimmed as cowski described.

The newer Untrim command has the capability of doing the same thing, except on a body with Sewn surfaces (so you can Untrim a solid face) and it's associative. Untrim essentially does the Extract Face and Remove Trim all in one step, regardless of the type of body.

Regarding the difference between Untrim and Enlarge, I'd have to say that Enlarge is different than Untrim in a couple of ways. First, you cannot use Enlarge on a surface that is Sewn to other surfaces, nor on a solid body face without at least making a copy or Extracting. Also, Enlarge allows you to shrink a surface's area, whereas Untrim only expands the surface but without any user input or control as far as how much to increase the surface's area.

I hope all that makes sense.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

Some people are like slinkies....they don't really have a purpose, but they still bring a smile to your face when you push them down the stairs.

 

[JohnRBaker]

I think Cowski is on the right track. Even a surface that is not a feature could be considered as trimmed since internally a surface is defined as some, usually rectangular, defined area or 'realm' with a set of boundaries. Now if the boundaries match the 'edges' of the defined area, then it's considered an untrimmed surface, but if the boundaries do not, than it's 'trimmed'. All that the 'Untrim' command does is to return the surface back to where the boundaries match the defined area. Now the thing to remember is that an Untrim operation can't create a surface LARGER than the original mathematical or defined area. This is not true with Enlarge which can force the size of the surface to extend past where the original math ends, but of course sometimes with some surprises for complex doubly curved surfaces and such. Canonical surfaces, such as planes and cylinders are better behaved, but complex free-form could become degenerate if extended (enlarged) too far past where the defined math ended.

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/

 

[hudson888]

Okay
Some surfaces are B-Surface types and some just aren't planar surfaces are one example and NX also supports other surface geometry which is less frequently created by surfacing with NX that it is by translators bring in IGES for example. Enlarge surface does not necessarily respect that original surface geometry, whereas removing the trim does. However removing the trim may, as already mentioned, reveal that the original surface was still smaller than you require.

The is another function that can create surfaces larger that the original which is Isoparametric trim/divide. You are changing the surface geometry somewhat, but the surface internals are based on the original so the change may be minimal or at least more controllable.

Lastly there is trim and extend which I will only say does a fine job of extending one or more surfaces to a larger boundary, but does not necessarily respect the original surface geometry either. Nor or the internal edge to edge conditions always ideal. If you really want convenience and don't care overly about the surface geometry then this may be the tool for you.

Lastly you can create extension surfaces as separate sheet bodies and sew them to the original sheets if they don't trim large enough. Of the tools for doing that Law extension is probably the best. A law extension can be generated tangentially from trimmed or untrimmed edges of single or multiple surfaces, which is where it has the advantage over the other surface extension. This is great for creating extended shut lines for tooling or engineering surfaces that may be based on a styling release.

If you are unaware of it it can do harm to a styling surface if you mess about with the geometry. By all means take the trim off if you need to, but beyond that ask somebody if you are unsure.

John,

Any reason why we can't simply extend a planar or other regular surface type such as a cylinder without turning it into a B-Surface which is thereafter treated as inferior as regards mating etc. The geometry is simple therefore it begs the question why the work process is not?

BTW I know there will an answer in the technical background but I'm not interested in that. I just want it to create a planar untrimmed rectangle that I can pull wider and trim back to suit without having to do a bunch of extra steps. the temptation at present is for some operators to take shortcuts and devalue the result often without due consideration for the consequences.

Best Regards

Hudson

 

[Xwheelguy]

Read the bold below and then what I posted above in the 3rd paragraph. I guess I'm not so far off the "right track" after all, at least according to the What's New for NX5 docs.

Untrim

What is it?

The Untrim command removes imposed boundaries. It extends planar, cylindrical, and conical faces in the linear direction of the selected face, and cylinders and cones along their axis.

With the Untrim command, you no longer have to extract multiple faces and then extend each of them. You can use the command to perform additional modeling tasks on a specific region of an existing model.

Where do I find it?

Choose Insert?Trim?Untrim.


I don't mind taking the credit if no one else is gonna give it to me. Absolutely no offense to my bud cowski intended at all.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

Some people are like slinkies....they don't really have a purpose, but they still bring a smile to your face when you push them down the stairs.

 

[hudson888]

Tim,

This might be what I'm asking John for, I'll have to dabble and get back about it.

in as far is it goes for free-form surfaces my earlier post will probably remain valid since a linear extension would be unsuitable in most cases.

Best Regards

Hudson

 

[JohnRBaker]

Hudson,

Any reason why we can't simply extend a planar or other regular surface type such as a cylinder without turning it into a B-Surface...?

About the best you can do is an 'Untrim' and hope that the face created is large enough for you task. However, that being said there is one more thing that will give something the might be good enough. Have you ever considered performing an 'Axisymmetric' Scale Body along either axis of Cylinder or a vector in the plane of the Planar surface?

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/

 

[hudson888]

Yes I reckon that you could do that, but whether you would save on the number of keystrokes is debatable. Was thinking more along the lines of the current enlarge surface except the the surface type could be ticked to original as is the case for extract surface. Having to do both is what tempts some people to cut corners, or maybe they just don't realize that planar surfaces extended that way aren't a planar surface type anymore. You'll often only find that out if you try to mate to it later on.

Best Regards

Hudson

 

[JohnRBaker]

But of course we can now create assembly constraints between b-surfaces.

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/

 

[hudson888]

John,

Can you then mate a flat planar underside of a bolt head or the flat face of a washer with a b-surface using the mate command?

Best Regards

Hudson

 

[JohnRBaker]

To start with, in NX 5, is you opt to use the new Assembly Constraints, there is no 'Mate' anymore but rather a single function which replaces Mate, Align and Tangent, and as such it should handle those situation where planar faces need to match up with non-planar faces, be whatever they are.

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/

 

[hudson888]

Thanks John,

That's two things I have to check out based on the one thread. Going well .

BTW, I'm using your NX-6 image as the desktop just to freak people out. See how many grab the spaceball .

Best Regards

Hudson

 

[cowski]

Tim,
You are correct, I was (unintentionally) referring to the Remove Trim command and not the new Untrim command. My apologies to all for muddling the conversation.

If I need a larger sheet body, my first attempt would be to adjust the defining strings. Sometimes this introduces unwanted side effects or is impossible (ie imported geometry). My second choice is "remove trim" (and now the new "untrim") since they are based on the underlying geometry. I consider "enlarge" to be the last resort since (as has already been mentioned) it can deviate from the original surface and can introduce self intersection or consistency errors.

 

[ewh]

Thanks for all of your responses! I think I have a handle on it now.

Believe it if you need it or leave it if you dare. - [small]Robert Hunter[/small]

 

[hudson888]

Tim,

Tried and liked the new un-trim command. It seems likely to serve well in most cases though perhaps not all.

John,

You encouraged me to look at the new component constrains as opposed to mating. I see that they resemble something that I've seen elsewhere and appear to work quite well. I haven't has time to test degrees of freedom as compared with mating so I don't yet know the state of play there. Apart from that the method you described works well and adds to the armory of things we could now do that we couldn't previously, but it seems to come at some price.

Why oh why do they have to be completely separate from mating and in fact to cancel out your ability to even have mating co-exist with them. I can't see the need for this based on a straight comparison between the two. Please consider if there isn't still time to implement the capacity for current mating conditions to be redefined automatically as new assembly constraints. I really think that all the methods available to mating need to be carried over to constraints and that a direct translation ought to be possible.

I guess there is a technical reason that enabled you to introduce the new functionality earlier I would take that as read. What I see is two tools where there ought to be one and a compromise that I'm disappointed with.

Best Regards

Hudson

 

[JohnRBaker]

To start with, you CAN convert Mating Conditions into Assembly Constraints and we have pretty much everything covered.

As for mixing and matching, it's just NOT possible, period. The old Mating Conditions were order dependent, much like a history-based feature model that plays back a recipe or tree, while the Assembly Constraints are more like the sketcher were the relationships are solved as a series of simultaneous equations. The order of creation is not important and if a change is made the entire model is resolved, just like a sketch (which is why sketches are created in a separate task environment).

Not sure what you mean by seeing multiple tools where there should be only one? If you're referring to having BOTH Mating Conditions and Assembly Constraints available, that will be resolved soon enough.

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/

 

[hudson888]

John,

Okay my mistake if I'm wrong but how CAN I convert mating conditions to constraints? If it is possible without re-selecting anything then I hold NX in high esteem. Even more-so if degrees of freedom and the sort expression driven simple motion that I used for the engine are also possible. In that case I'd be on-board to simply say out with the old and in with the new .

Best Regards

Hudson

 

[wmalan]

Untrim is one of THE main tools us nc programmers use almost every day. We create a linked wave sheet body then untrim to use as the part surface so the tool can flow beyond the enxtents of the part without rolling over.

--
Bill

 

[JohnRBaker]

OK, some ground rules.

First, we do not attempt to automatically convert Mating Conditions into Assembly Constraints when an old assembly file is opened in NX 5. Even though all of the parts get their internal data structures upgraded when an older part is opened in NX 5, this is NOT done with Mating Conditions. There are a couple of reasons for that, such as when an assembly file has been released and there's no need to make any further changes to the assembly, there is technically NO need to do a conversion since while it is true that you can't mix Mating Conditions and Assembly Constraints in the same part file, there are no problems having an assembly created with Assembly Constraints which contains sub-assemblies created using Mating Conditions. This way users can take existing released sub-assemblies and reuse them in their latest assemblies.

Now as to how one goes about actually converting a pre-NX 5 assembly so that the Mating Conditions are upgraded to Assembly Constraints, you must first switch NX 5 over so that Assembly Constraints are now the default scheme. You can do this in Customer Defaults -> Assemblies -> Positioning -> Interface and set the Positioning option to Positioning Constraints. Note that once this has been set, when you launch NX and open a file, on the assembly toolbar the Mating Conditions icons will have been replaced with Assembly Constraint tools. Note that you can temporarily set the system, at least for your current session, back to Mating Conditions, by going to Preferences -> Assemblies... and set the 'Assembly Positioning Interaction' option.

Now, with the system set to Assembly Constraints, open your existing pre-NX 5 assembly (you can use partial loading if you wish) and once open, simply select the 'Assembly Constraints' function either from the Assemblies pull-down menu or the Assemblies toolbar. After selecting the function a warning message comes up telling you that the assembly contains Mating Conditions and asking whether you want to convert them or not (note that you can ignore this message and continue leaving them in place and build new constraint on top of the old ones since these schemes totally ignore each other like they were never there, but it is confusing so I'm not sure I would recommend that anyone work that way or even try to). If you select the convert option, a dialog will come up which offers some options like only converting the Work Part level only (ignores the internals of any sub-assemblies), or the Work Part and any open children, or Work Part and all referenced parts (which means that it will automatically open any unopened yet referenced part files). Also there are some options about whether you want to get a summary or a full report afterwords, etc.

Anyway, I just tested this on a modest assembly, 160 components in 3 files (the main assembly and 2 sub-assemblies) which was modeled in Unigraphics V14.0 and last updated in Unigraphics V17.0 a bit over 7 years ago. The conversion took maybe 45 seconds and 333 constraints were converted with no errors.

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/