Show and Hide Alternative 1

[neshom]

I am using Show and Hide option to hide objects like Datumn, Curve, and Sketches. It works, but it is very temporary as when I edit some of the parts and switch back to the assembly, the hidden objects are back again.

What is the best permanent approach (reference sets, layers, etc) for only showing what one needs?

Thanks

 

[lohiths]

Use layers, use any one layer for only datum's or curves, and switch off that layer in assembly file
or
create a reference set named as solid body in part file, add only solid bodys. and change reference set to solid body of the part in assembly tree structure by right clicking the part.
or
you want to hide all layers or carves use selection filters its available in top of left with pull-down button.
or
u can use ctrl+w to hide and show

 

[NutAce]

NX out of the box already has a number of layer categories (Sketches, Datums, curves) where you can place your entities...
By switching them on and off you can permanently either show or hide the contents...

You don't need to create a reference set. NX out of the box already has a reference set called model...this will automatically contain the 3D geometry you create. Make yourself familiar with the usage of reference sets...Reference sets are used to show or hide geometry in context of an assembly.

Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2
HPZ420 Intel(R) Xeon(R) CPU E5-1620 0 @ 3.60GHz, 32 Gb Win7 64B
Nvidea Quadro4000 2048MB DDR5

HP Zbook15
Intel(R) Core(TM) i7-4800MQ
CPU @ 2.70 GHz Win7 64b
Nvidia K1100M 2048 MB DDR5

 

[neshom]

Thanks for your replies.
I know that Show and Hide is a temporary solution and it changes after editing parts or for new parts. So the question is that:are reference set or layers are permament solutions? And do you need to set them for each and every single part in an assembly?

Also, I have read several advises against using reference sets in assembly, e.g.:

http://www.eng-tips.com/viewthread.cfm?qid=308516

Do you recommend against this? I've read that reference sets are good only for parts and not for assembly or subassembly. If this is the case, then again do you set reference sets for indivitual parts or it is just one time process that does it for all parts in an assembly?

Thanks

 

[cowski]

Reference sets are created in the part, but they don't come into use until you add the part as a component in another file. When you create a reference set in a part, you specify which objects to add. Only the objects that you add will show up in the assembly when the reference set is used. In this way you can filter out the construction geometry when displaying a component in an assembly. Using reference sets to filter out part geometry for display in an assembly is considered "best practice".

Since an assembly is also a "part file", reference sets can be defined in the assembly part. Multiple reference sets can be created with different combinations of components in each. Some use this ability to create "configurations" or "variations" of assemblies. However, this is considered poor practice as it can cause some unforeseen problems downstream. The preferred method to create such configurations is to use "assembly arrangements"; which allows you to suppress and/or re-position components.

www.nxjournaling.com

 

[neshom]

Thanks for your reply.

The thing is that with layers, you have to first move all of the objects that you want to hand or show to specific layers, and then try making them visible or invisible. Or maybe, right ate the time of creating every single objects, change the work layer so that they move to their own categorized layers. This, I imagine, is a great practice for the components that will be used for a long time under multiple revisions. However, if you are designing a one-time-design part that there won't be any major future modifications, it may not justify the time that you need to spend to move (even using fast filtering techniques) to sort all of the objects. So, I believe, using layer to hid and show different category of objects in an assembly is not a practical solution especially for the cases that new parts will be added and you have to first sort their objects into your layers in order to be able to use the layers for properly hiding and showing what you want.

So, the questions are:

1) Is there anyway to make the layers to automatically update and move the objects to their own category? This way you don't need to keep sorting new object and new parts with lots of unsorted objects.
2) Is there any solution to permanently hide/show for example Datums (existing Datums and all that will be created later in the design process) - without being worry about the layer of the obejcts and sorting the new objects?

 

[NutAce]

So, the questions are:

1) Is there anyway to make the layers to automatically update and move the objects to their own category? This way you don't need to keep sorting new object and new parts with lots of unsorted objects.
2) Is there any solution to permanently hide/show for example Datums (existing Datums and all that will be created later in the design process) - without being worry about the layer of the obejcts and sorting the new objects?

1) No. You need to program that yourself (NX open)
2) Reference sets (when in context of an assembly) or when in context of the part itself you can use the Blank (ctrl-B) option...

Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2
HPZ420 Intel(R) Xeon(R) CPU E5-1620 0 @ 3.60GHz, 32 Gb Win7 64B
Nvidea Quadro4000 2048MB DDR5

HP Zbook15
Intel(R) Core(TM) i7-4800MQ
CPU @ 2.70 GHz Win7 64b
Nvidia K1100M 2048 MB DDR5

 

[neshom]

Reference sets are created in the part, but they don't come into use until you add the part as a component in another file. When you create a reference set in a part, you specify which objects to add. Only the objects that you add will show up in the assembly when the reference set is used. In this way you can filter out the construction geometry when displaying a component in an assembly. Using reference sets to filter out part geometry for display in an assembly is considered "best practice".

Since an assembly is also a "part file", reference sets can be defined in the assembly part. Multiple reference sets can be created with different combinations of components in each. Some use this ability to create "configurations" or "variations" of assemblies. However, this is considered poor practice as it can cause some unforeseen problems downstream. The preferred method to create such configurations is to use "assembly arrangements"; which allows you to suppress and/or re-position components.

I am sure, this works. However, this need the user to create Reference Set for new parts and also set the Reference Sets for every single parts in the assembly. So, to show only solids in the assembly, the user needs to set the relevant Reference Sets for all of the parts in the assembly and sub-assemblies. If he want to show all of the Datums, the user then needs to change the reference sets for all of the parts, and so on. This is only true if the user has already set the Reference Sets for all of the existing and new parts. Am I right or I am missing something here? (I am a new user switching from SW. In SW, you can easily and simply turn different objects On and Off and they stay that way until you change their visibility. I am sure that Reference Sets are extremely powerful for doing lots of tasks. However, I only need to show and hide different objects and nothing more at this stage.)

Any suggestion?

 

[neshom]

1) No. You need to program that yourself (NX open)

That's right, but even using NX Open you will end up with a button (or even a keyboard shortcut) which you have to constantly execute in order to sort the new objects to their layers. So, if using layers or reference sets are the only solutions, then my question is how to effeciently manage them in a way you spend least time sorting the objects in the layers and hiding and showing layers and also creating and setting the reference sets?

All I am trying to find is an efficient way of for example hiding all of the existing and NEW Datums in a way that you don't need to keep doing another task in order to keep the new Datums hidden or visible (only one-time method). Any suggestion?

 

[cowski]

I am sure, this works. However, this need the user to create Reference Set for new parts and also set the Reference Sets for every single parts in the assembly. So, to show only solids in the assembly, the user needs to set the relevant Reference Sets for all of the parts in the assembly and sub-assemblies. If he want to show all of the Datums, the user then needs to change the reference sets for all of the parts, and so on. This is only true if the user has already set the Reference Sets for all of the existing and new parts. Am I right or I am missing something here? (I am a new user switching from SW. In SW, you can easily and simply turn different objects On and Off and they stay that way until you change their visibility. I am sure that Reference Sets are extremely powerful for doing lots of tasks. However, I only need to show and hide different objects and nothing more at this stage.)

You are both partly right and missing something.

NX has an option to automatically maintain a reference set for you. With out-of-the-box (OOTB) settings, this is the MODEL reference set; solid and sheet bodies only will be placed in it automatically. Sketches, datums, curves, etc will be filtered out automatically. You can specify which reference set to use for every component in your load options. There are some options in the customer defaults to tailor this automatic reference set to your needs.

Also, check your assembly preferences. In the "work part" section, there is an option to "display as entire part"; when you make a component the "work part" this will automatically switch over to the "entire part" reference set which will cause a lot of construction geometry to become visible. I prefer to have this option turned off as it allows me more control of what gets displayed and when it gets displayed.

www.nxjournaling.com

 

[neshom]

NX has an option to automatically maintain a reference set for you. With out-of-the-box (OOTB) settings, this is the MODEL reference set; solid and sheet bodies only will be placed in it automatically. Sketches, datums, curves, etc will be filtered out automatically. You can specify which reference set to use for every component in your load options. There are some options in the customer defaults to tailor this automatic reference set to your needs.

Thanks for your comment. I tried this, but it is not helpful. Here is what I am facing:

In my assembly I use Show and Hide to hide all datums, sketches, and curves. It looks good now. I then select two or three of the components and run the command Show only. This hide all of the un-selected parts. Now, if in assembly navigator I right click on Assembly and run the Show command, it will show all of the parts of the assembly as well as all of the datums, curves, and sketches. Am I doing something wrong here? I only need to show all of the components just like it was before running Show Only command.

Thanks in advance.

 

[Xwheelguy]

Go into each component file and see what belongs to the MODEL Reference Set - if you have Datums, etc. showing highlighted when you click on the Reference Set, then you need to remove them from the Reference Set. If they don't belong, then you need to go back into the assembly and set your Reference Set to MODEL in the Assembly Navigator.

Reference Sets work in an assembly context just like they've been described in previous posts - if you're having issues, then you're missing a step somewhere.

I understand what you're desiring but the simple fact is that without custom programming, you're going to have to manually manage these entities, more than likely with a combination of Layers/Categories and Reference Sets. GM has been doing it for decades in NX, so it works if you can get your head around it all. Manually moving things isn't as bad as it seems at the component level if you utilize NX's Preselection Filters.

Tim Flater
NX Designer
NX 9.0.3.4 Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

[neshom]

Go into each component file and see what belongs to the MODEL Reference Set - if you have Datums, etc. showing highlighted when you click on the Reference Set, then you need to remove them from the Reference Set. If they don't belong, then you need to go back into the assembly and set your Reference Set to MODEL in the Assembly Navigator.

Thanks for your comment.
The objects do not belong to any component as they are in the assembly prt itself. I needed to use hole series and for that I created some sketches and datums. In what Reference Set I need to hide them?

 

[NutAce]

The objects do not belong to any component as they are in the assembly prt itself. I needed to use hole series and for that I created some sketches and datums. In what Reference Set I need to hide them?

That is not how reference sets work....
A reference set is created in a part. when that part is used in an assembly you tell the assembly to use for that part the reference set it has. When you have multiple reference sets in that part you can pick the one which shows you the correct information you need in the context of your assembly.

a reference set can not be used to show and hide geometry in the part itself where it has been created. Reference sets work (only) one level up in the assembly where the part has been used as a component.


Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2
HPZ420 Intel(R) Xeon(R) CPU E5-1620 0 @ 3.60GHz, 32 Gb Win7 64B
Nvidea Quadro4000 2048MB DDR5

HP Zbook15
Intel(R) Core(TM) i7-4800MQ
CPU @ 2.70 GHz Win7 64b
Nvidia K1100M 2048 MB DDR5

 

[titusnico]

Hi all .

I'm new on this website. I search the 'Siemens: UG/NX Forum' to find an answer to my question and this topic seems to be the one where I should post.

I'm using NX10 software and I can prepare a part with a reference set that contains two solid bodies : one visible and one hidden.

Now, when I add my part as a component of a parent assembly, I select the prepared reference set in the part. I was hoping the original visibilities set in the part file would be respected in the assembly file but it is not the case. The two solid bodies become visibles in the assembly !

One more surprising thing is that you can do (after having change the type filter to 'Solid Body') a right-click on the first solid body, then the sub-menu allows you to 'Hide' it. It works and there is nothing strange here but if you do the same on the second solid body the sub-menu allows you to 'Show' it whereas it is already displayed. This last command does not change anything, the second solid body stays visible and its visibility status does not change. With the presence of this 'Show' command in the sub-menu, does it mean that the visibility status is set as 'hidden' on this second solid body but the graphical window does not follow this status ?

Is that a bug of the software ? I mean, shouldn't we have only one visible solid body added in the assembly in my case ? I know that the second solid body can be hidden with Ctrl + B keys but I was expecting that NX will do this for me, am I wrong ?

Nico.

 

[titusnico]

It's me again.

I think I understand : the visibilities are only effective in their own context. When you add the component reference set contents in the parent assembly, it takes the whole contents of the reference set regardless of the visibilities set in the part context. You can, then, set other visibilities in the assembly context if you want.

But it still does not explain the 'Show' item in the right-click sub-menu...

Nico.