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Frustration....I could do this in solidworks but can't seem to do it in NX!?

Experimenter
Experimenter

My first ever post here on this forum and I seemingly have an issue that I cannot believe there's not a solution to in NX as on paper its a far more powerful system than my previously used software.

 

Anyway as quick as I can. I have a component made up from three individually machined parts which are then held in a jig and hard soldered (brazed) together.

 

So I had three individual components (with their drawings) and an assembly (again with a drawing).

 

After making some prototypes it's apparent that some of the machining operations need to be done after brazing, just a couple of slots that run through the three parts. So I'm thinking simple remove the slots from the individual parts and do an assembly cut at the top level.

 

Thing is I want just one top level assembly drawing showing the semi-machined parts with brazing instructions and then (say on a second sheet) the post brazing machining.

 

I'm thinking as it's an assembly I will be able to create a 'brazed' arrangement and a 'fully machined' arrangement.....just suppressing the assembly cut in the first!?

 

Doesn't give me the option....which is disapointing. I really don't want to go down the route of introducing another level (so a brazed assembly drawing AND a final machining drawing.....that's a bit nuts.

 

I don't want to refer to oother softwares by name (not on this forum) but one I had used for years I could have very easily done this through configurations....absolutely no problem.

 

What can I do???

 

Sorry to go on a bit...especially a first post.

 

Cheers.

 

Gazza

 

9 REPLIES

Re: Frustration....I could do this in solidworks but can't seem to do it in NX!?

Gears Phenom Gears Phenom
Gears Phenom

Pssst...the other software is in your subject Smiley Happy  I've been working with a few people moving from SW to NX.

 

That said, I've done this by wave linking the solid bodies that will get cut at the assembly level, in my assembly drawing (I'm assuming you are using master model, with seperate model, and drawing files).  Then make sure these wave link bodies are on a different layer than your components.  Now, add the before-cut views, by taking them from the drawing, and not the model.  This bit is tricky/confusing for some, but in this section of the dialog, you can pick where the view is coming from:

viewfromdwg.jpg

 

Then, use visible in view, to turn on the layers with the wave link bodies, and turn off the layer(s) with components.

 

Maybe be other ways to do it, but from what you've said, this should work.  

-Dave
NX 11 | Teamcenter 11 | Windows 10

Re: Frustration....I could do this in solidworks but can't seem to do it in NX!?

Phenom
Phenom

Don't even think that you have worked before with Configurations, Weldments etc. You don't find such robust systems in NX. So just forget about them.

 

Majority of NX users follow their pioneers and their systems, which have evolved from 2d era and just by having the 3rd dimension could satisfy them thoroughly. You will find "Layers" in 3d model (which I consider as a 2d evolutionary leftover) and it’s a world to them.

 

You should remember that NX is a high end OEM focused product and highly capable of constructing unique products from scratch for their needs. So what I felt was, that it’s kind of distant from efficiently supporting day to day manufacturing work, doing same kind of work daily. Just look at how difficult it is to make a drawing from your model! You could make a drawing inside your model or at the same time create another driven part and name it as a drawing; a Master Model Drawing. BTW, with MMD system, the master i.e. the model doesn’t know that it has a child drawing! If you want to clone (= pack’n Go) you will have to select them manually. Isn’t it quite messy at manufacturing level?

 

As I said before, you should forget the past and be happy with what you got now and go with the flow. Good luck!

Michael Fernando


Die Designer
NX 11.0.2.7 + PDW

Re: Frustration....I could do this in solidworks but can't seem to do it in NX!?

Legend
Legend

Hi,

 

You couldn't make it in NX does not mean that it can not be done in NX. The only thing you need to figure out what is the best way to do it in NX for your type of application as NX has different ways to achieve the same thing.

 

I would suggest not to compare any 2 softwares for same application, it will give you nothing but frustration.

 

Are you sure that the things you had done in the past is the best/correct way of doing things becaues that was possible in your old software and the same method is not in NX?

 

When it comes to creation of Design definitions and Manufacturing definitions, every organisation needs to define the best process following engineering standards, separating both definitions to manage the data and data change efficiently.

 

 

All the best!

Re: Frustration....I could do this in solidworks but can't seem to do it in NX!?

Siemens Phenom Siemens Phenom
Siemens Phenom

Hi Gazzachap,

 

What you are asking for is certainly possible in NX. What dictates what method you use is what license you have available to you. In my attached movie example I assume that you have a standard NX licence and no Teamcenter backbone. When it comes to process modeling I highly recommend to NOT cut corners and actually define parts in separate files as they are processed. Combining processes in order to “save” number of files can be fine BUT often come back to bite you when it comes to configurations down the line. Combining processes into one file can be OK if it is a simpler product and configuration – this is a judgement call on your behalf.

 

In the movie file there are 3 components assembled together into one assembly. The in the assembly contained components are the deliverables of each incoming component. There is a drawing file (master modeling concept) of the assembly as well where the target is to show the process stages "110-Incoming_Clamped_Geometry-nBrasing” and “120-Key_Seating_Machining” on 2 different drawing sheets. In the assembly the parts are clamped (note really shown – just positioned together in relations to each other). WAVE links are used to associatively extract information into the assembly enabling to show 2 different versions, mentioned above, of your assembly. Layers and reference sets are utilized in order to filter geometry on the drawing. Visible in View enables to turn on or off geometry to be shown in various views on your drawing.

 

Note that this is targeted to keep number of files to a minimum BUT I would recommend either to create a working structure or up your WAVE license enabling wave links to exist without supporting assembly structure (as this might cause issues with configurations down the line depending on your products downstream complexity)

 

Have a look at the movie file to get an idea of a potential process. i hope this help you a bit.

 

Best Regards

Fred

 

(view in My Videos)

Re: Frustration....I could do this in solidworks but can't seem to do it in NX!?

Phenom
Phenom

Hi @Gazzachap,

I was a SolidWorks user for 11 years. Configurations into NX doesn't exist.

I don't suggest solution like @Sandman for some reasons :

  1. very complicated process, which must be maintained and made to understand also to the colleagues in case you work between colleagues
  2. The part need to be managed with reference set, otherwise in the assemblies that use it, you'll see everything
  3. The weight part is replicate for each body, see in the weight column in the ANT (Assembly navigator)

Make life simple, also in the NX projects. NX doesn't have configurations, accept its faults and its merits, for each process you creat a part and in the drawing, like in SolidWorks you can add view from main part or different parts.

Thank you...

Using NX 11 / RuleDesigner PDM

Re: Frustration....I could do this in solidworks but can't seem to do it in NX!?

Siemens Phenom Siemens Phenom
Siemens Phenom

Cubalibre et all,

 

The method shown is based on the assumption that the license file is for basic NX without the support of the advance capabilities of WAVE. As mentioned there are several ways of going about this - one is a control utilizing a structure (that for configuration purposes always should be in place when working with interpart links without the support of a PDM-system - and I would still use it even within a PDM system). The purpose here is to quickly give an idea of what you can do to and to show some of the tools available in doing so - at the end of the day it all boils down to your company’s process flow... All your bullets would be addressed with that control structure.

 

 

Best Regards

Fred

Re: Frustration....I could do this in solidworks but can't seem to do it in NX!?

Phenom
Phenom

@Sandman wrote:

Cubalibre et all,

 

The method shown is based on the assumption that the license file is for basic NX without the support of the advance capabilities of WAVE. As mentioned there are several ways of going about this - one is a control utilizing a structure (that for configuration purposes always should be in place when working with interpart links without the support of a PDM-system - and I would still use it even within a PDM system). The purpose here is to quickly give an idea of what you can do to and to show some of the tools available in doing so - at the end of the day it all boils down to your company’s process flow... All your bullets would be addressed with that control structure.

method shown is based on the assumtion that the licensfile is for basic NX without the support of the advance capabilities of WAVE. As mentioned there are sevevral ways of going about this - one is a control utilizing a structure (that for configuration purposes allways should be in place when working with interpart links without the suppor of a PDM-system - and I would still use it even within a PDM system). The purpose here is to quickly give an idea of what you can do to and to show some of the tools availabe in doing so - at the end of the day it all bouils down to your companys process flow... All your bullets would be adressed with that control structure.

 

Best Regards

Fred


Hi @Sandman,

this is your point of view, for me, as NX designer, it's strange, imaginative, very articulate, inefficient and distorting the functionality of NX.

You need to simulate machined processes ? Indipendent to the license, one part file for each process. This is the right solution, simple, efficient and for everyone.

Thank you...

Using NX 11 / RuleDesigner PDM

Re: Frustration....I could do this in solidworks but can't seem to do it in NX!?

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor


You need to simulate machined processes ? Indipendent to the license, one part file for each process. This is the right solution, simple, efficient and for everyone.


To be fair, that was @Sandman's original suggestion:

 

"When it comes to process modeling I highly recommend to NOT cut corners and actually define parts in separate files as they are processed."

Re: Frustration....I could do this in solidworks but can't seem to do it in NX!?

Solution Partner Valued Contributor Solution Partner Valued Contributor
Solution Partner Valued Contributor
Gazzachap, Just a quick question for my own curiosity's sake and by no means implying anything about you, your abilities or knowledge, or the value of your experience... have you ever had formal training in NX?