Huge Project and Whole Drafts to Update (How?) 9

[3vans]

How do you do guys,
First of all I found this site very helpful but I couldn't find any useful tips on my issue; thus I am posting my problem here in this forum, hoping somebody assist me to handle it.

I was working on an NX project for the last two months, a few days ago I have manipulated and changed some of the models, no problem so far; I had changed and then exported my project's drafts one by one. After finalizing the project I've noticed those intricacies I had made earlier were not applied to the drafts. Now I have to update each and every draft in the project and export it again. why is that so difficult? The solution is a bit pain in the neck, sorry for that but I am spending my day to update those outdated drafts and still, I'm almost at the beginning.

Help me please, is there any other way to handle the issue in the NX software?

thank you so much,
Michael Evans,
Regards

 

[moosaviamir]

Same problem here...

 

[moosaviamir]

Hello 3Vans
It seems there are more people out there having the same problem!:|
Old post having the same problem

Dear 3Vans let me know if you found any solution!

 

[Toost]

I am trying to understand what's going wrong for you, help me understand,:
exported the drafts, - exported ?
You "had changed and then exported my projects drafts" - how can the drafts then not be up to date ?

Regards,
Tomas

 

[JohnAB9]

Dear 3vans,
This is a huge burden to handle.
I myself was buckled with this problem we all did it manually.
unfortunately there aren't any automation involved with this process.

 

[3vans]

Dear Toost,
Check it out yourself!
1- Create a simple object
2- Start Drafting by making a 3 view draft
3- Back to modeling and make a hole or something on the object.
4- Back to drafting and Boom!!! there is some unwanted lines you don't wanted to be there!

There you go, you have to update that draft, for small projects this is ok but my project is consist of more than 100 files. this issue drives me totally crazy!

 

[3vans]

to moosaviamir: I'll let you know about the issue.
to JohnAB9: didn't you figure it out? there aren't any journal or sth like that at all?

Dear All,
if an image would help, just notify to upload it.
I appreciate your concern and thanks you.

 

[moosaviamir]

Here is some pictures
Before change:

After change:

how to update:

Seems really easy? try it with a 1000 part project...

 

[JohnAB9]

nope , I could not find any journal . I,ve marked this post in my archives please post the solution here if you find any ,
and I hope you will find it soon.
BTW problem illustration through an image will help other professional to better understand this pain in the *** !!!!!
thanks to moosaviamir

Zai gezunt

 

[ewh]

Drawing views have always needed updating whenever there is a model change, and I would rather update the drawings than assume that the software knew what I wanted to see.
That said, it wouldn't suprise me if someone has a journal or other method to automate the process.

“Know the rules well, so you can break them effectively.”
-Dalai Lama XIV

 

[FrankSwinks]

Here is a first journal to update drawing views. I have kept it very simple at this stage in that it works on just the current work part. It cycles through all drawings of the work part and updates all views. It certainly can be improved significantly by checking a drawing sheet to see if any views need updating. Only if required should they be updated. Also it is a simple addition to cycle through the component parts of an assembly to do the drawings update.

Option Strict Off
Imports System
Imports NXOpen
Imports NXOpen.UF
Imports NXOpen.Drawings

Module UpdateDrawings
    
    Sub Main()
        Dim s As Session = Session.GetSession()
        Dim ui As UI = ui.GetUI()
        Dim ufs As UFSession = UFSession.GetUFSession()
        Dim wp As Part = s.Parts.Work
        Dim drawingsheets As DrawingSheet()
        drawingsheets = wp.DrawingSheets.ToArray
        ' ----------------------------------------------
        ' Here we loop through all the sheets in the work part.
        ' For each sheet, we open the sheet, update all views in it.
        ' ----------------------------------------------
        For Each aSheet As DrawingSheet In drawingsheets
            aSheet.Open()
            wp.DraftingViews.UpdateViews(DraftingViewCollection.ViewUpdateOption.All, aSheet)
        Next
    End Sub

    Public Function GetUnloadOption(ByVal dummy As String) As Integer
        'Unloads the image immediately after execution within NX
        GetUnloadOption = NXOpen.Session.LibraryUnloadOption.Immediately
    End Function

End Module

Frank Swinkels

 

[3vans]

Dear All,
As I promised earlier for sharing th solution in case I found it here you are.
I have googled for "NX draft updating problem" and I found this, by following the links I found this video, here. Finally I could download the add-in here on KeenCAD.com and amazingly it worked (an almost freeware that actually works for just 10 box).
I've purchased the other add-in and I think it just saved my week ahead.

to FrankSwinks: thanks for your concern, I dig it out and I've used the above-mentioned add-in; of course I appreciate your hint, but this add-in saved me. btw I don't think that this is just a simple journal, cause this program updated each part and every file in a given folder

Best Regards,
Michael Evans

 

[3vans]

it is four in the morning and I'll pass out soon. hope tomorrow I earn my boss' trust more than ever as he wouldn't expect that this project will be finalized anytime sooner than next monday.

Thank you all, and I appreciate your concerns.

 

[jerry1423]

You can set the drawing views to update automatically when the drawing is open.
Preferences (pull-down) -> Drafting -> View -> uncheck "Delay View Update"

 

[WilsonYau]

I might have done something wrong, if so please correct me.
But what jerry1423 suggested only partially works. I tried what he suggested by making a part file of a simple block, then created a drawing of the block on a separate file. I then added a through hole in the middle.
The drawing did update itself but the same unwanted lines, as shown by moosaviamir, still showed up on my drawing. Any fix?

 

[moosaviamir]

Thank you 3vans for sharing your result!
I did check out trial versions and it was really good.
3vans did you buy add-in's? can i trust them?

 

[JohnAB9]

Who are you? what are you? a humanoid perhaps? working on a project till 4 am? and then posting about it here? your devotion to perfection is awesome.
I saw the youtube videos it was brilliant, are you sure about the results? are these add-ins reliable?
and one more question to ask, what do you mean by "btw I don't think that this is just a simple journal"?

Zai gezunt

 

[3vans]

to moosaviamir: sure but the payment was a bit different, first I paid ten box using my credit card and then posted the information on the payment form, why? I don't know! nevertheless the fee was not that much to hesitate, after a little while I've got an email that included the software and instructions to register it.

to JohnAB9: ha ha ha ha ha, I overslept this morning, and I was late but when I presented the finalized project jaws was :O
about your question I don't know it was a bit different but in an effective direction!!!!!

 

[Toost]

Hold it a second,
in the three images above, "The unwanted lines": , May i assume that 1) this is the sketch and not edges of the solid body ? and 2) ( not assuming) this drawing is made inside the same file as the model .
Then 1 If you desire to care for "curves" in the drawing view, there is an extra option under the hidden line options, "Include model curves", which is off by default. the reason for the off state is that NX will need extra computing time if we mix the object types, and performance is a big desire. So yes you can mix object types but it will take longer time to compute hidden lines.
If you desire so you can have the extrusion hide the sketch, ( Make Sketch internal) and it will not display elsewhere. Both as a default setting and a per feature definition.
Or, if you work with other types of features which doesn't have the "make internal" option, the standard procedure is to move the curves/ sketch to a hidden layer.
then 2 If the model and the drawing would have been in different files, the automatic reference set handling would have had excluded the sketch from displaying on the drawing.
Model and drawing in separate files is the recommended practice since at least 15 years.

The tip from Jerry1423 does work ( if you also follow what I wrote above), all you need to do is display the drawing/save/plot. The setting is part-specific and will be stored with the part. You can also set this in the customer defaults for future files.
The reason it is delayed by default is if your models are complex and the updating therefore takes notable time, It might in those cases not be desirable if NX starts updating as soon as you display the drawing.

If one desires to update drawings in batch mode, one can do that by using the Refile utility. There is a specific option to update drawing views. ( Refile will re-save the file after the update has finished.

I don't see the fuzz.

Regards,
Tomas

 

[Toost]

Hm, Three new names in this thread. Similar vocabulary. References to a site where no one dares to write his/her name. Pictures showing the Siemens template.( That somebody created a model in)

F..k, why was i trying to be helpful?