Drawing files automation

[symphony123]

I happen to work in NX and looking for a way to automate drawings for similar kind of part files. Is there any way to achieve this either through Knowledge fusion or any capabilities within NX itself?

For example, I have different sizes for flanges and the parameters are already known I would put everything into part family spreadsheet and could create each part family member whichever I would want to.

But each time I have to create the drawings from scratch though the general scenario is that the drawings are almost 90% same for all the different sizes. Please advice if there is any way or capabilities within NX or Knowledge fusion where I can capture at least partial information or any generic drawing getting linked to all the parts automatically.

 

[hudson888]

If and only if it is a part family then I would create the drawing initially at least in the same part as the model. I would create all the part family members and then I'd probably rename the files as drawings and use create component to set them up as master model concept. It is a work around that requires some effort and some manual intervention, but it probably beats creating each drawing separately.

You don't have to split the part file and drawing according to master model concept but I probably would anyway. Sometimes it will relate to issues with file and data management in organisations, and other times just for the performance benefits of doing so.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[JohnRBaker]

What version of NX are you running?

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
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.

 

[symphony123]

I am working on NX 6

 

[JohnRBaker]

OK, you can use Part Families and the Master Model Drafting approach as long as you know how to leverage the capabilities of NX and have gotten things set-up ahead of time.

I have created a sample Part Family with a couple of the Family Members already created as well as a master drawing. Just download the file, edit the file extension from .zipper to .zip and extract the files.

The part file, 'Flange.prt' if the Part Family master template part (I've defined 6 parts in the family). The file 'Flange_dwg.prt' is the master model drawing file. When you wish to create a new 'Flange' model and it's accompanying Drawing, first open 'Flange.prt' and go to the Part Family spreadsheet and select the row of the part that you wish to create and then select...

PartFamily -> Create Parts

...and that member of the Part Family will be created.

Now open the Drawing file, 'Flange_dwg.prt', enter the Drafting module and go to the Assembly Navigator and select the flange component, press MB3 and select the 'Replace Component...' item. When the dialog comes up make sure that the 'Maintain Relationships' option in the Settings section is toggled ON. Now select the new Flange file that you wish to make a drawing of (you may need to select the 'Browse' icon if the part is not listed in the list of 'Loaded' files). After the drawing updates, select...

Edit -> View -> Update Views

...and the drawing would now be updated (you might need to tidy up some item like just selecting the bolt circle and any new holes that need to be included, as well as moving dimensions around to better locations).

Now just do a...

File -> Save As...

...and give your drawing a new file name. And there you have it, a new member of the Part Family and a Drawing of the part.

Granted, this is a simple example, but I think it demonstrates what is possible with NX. Note that what I did here could have been done with older versions of NX, certainly NX 4 or NX 5 (although the Centerline Bolt-Circle on the drawing my not have been able to update as easily as it does in NX 6).

Anyway, give it a try and see if this might inspire you to try something similar with your parts.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
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.

 

[uwam2ie]

Ok, thanks, John
nice example to show partfamilies an replacing component in master model concept.To expand the question. Is there a way use spreadsheets/attributes with external Excel spread sheet to control the attributes outside from nx?

 

[JohnRBaker]

Yes, there are Expression functions which can read the cells of a Spreadsheet. What I did was update the Drawing of the Flange example adding a note which is linked to an Attribute named 'Finish'. Then I created a simple spreadsheet, 'Finish_Standards.xls', which defines 5 different Finish call-outs. Then I created an expression which returns the value of the 'Finish' Attribute from the Spreadsheet based on which integer I enter as the value of an expression named 'aa_Finish_Number'.

To see how I did this, download the attached file, edit the file extension from .zipper to .zip before extracting the files. Now take the spreadsheet file and place it in your system's C:\ folder. Now open the Drawing file and see that I've updated the note on the face of the Drawing adding a line for 'FINISH:'. Now open the Expression dialog and edit the value of 'aa_Finish_Number' setting it equal to any value from 1 to 5 and selecting the OK button. Note that the Drawing text updates reflecting the new part 'Finish' callout.

Now if you wish to place the spread in some other location, you will need to edit the string representing the path to the spreadsheet contained in the Expression titled 'Finish_Att'.

If you wish to see what other functions can be incorporated into an Expression, open the Expression dialog and select the icon in the left-hand side of the dialog titled 'f(x)'. Select the 'Choose a Category' drop-down list to see all of the classes of functions which you can use. Go to the near the bottom of the list and select 'spreadsheet'. If you wish to see how to use a particular function, select it and a short description will appear below it. If you wish more information, select the Help icon '?' and a one page help document will be displayed.

Anyway, this should get you started.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
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.

 

[symphony123]

John,
Can you please advice me how do i select the flange component after i get to Assembly navigator.(in the drawing part file)
Enclosed is the attachment illustrating where I am trying to go ahead to select the flange component but could not find an option for that.
Please suggest.

 

[JohnRBaker]

You need to select the Component from WITHIN the Assembly Navigator itself, as shown below:

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
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.

 

[uwam2ie]

... how can I resize the sheet format that the titleblock and the frame is updated with minimum of rework on the new sheet.
thx in ad

 

[JohnRBaker]

There's no direct way to do this other than first removing the old border, editing the size of the Drawing Sheet and then manually adding a new border back in.

However, starting with NX 5 there is an interesting alternative approach (which I just tested and it does work).

With the introduction of the built-in, Template-based File-> New function, we also included a scheme whereby you could add additional drawing sheets also using templates.

Now you have to have already set up a series of Second-Sheet templates (I created my own XML file which adds an additional tab to the Resource Bar giving access to a set of pre-defined second-sheet Drawing templates) but if you do all you have to do is add that second sheet selecting the template which gives you the desired new size for your drawing.

Once that second sheet, along with it's own drawing border has been added, all you do is go to the Part Navigator, open the section which shows the drawing views on 'Sheet1' and simply drag them all to 'Sheet2'. Now if your new drawing is larger than the original, there should be no problems, but you may still wish to manually move the views to more appropriate locations on the second sheet once they've been moved there so that the drawing still looks good and there is adequate space around the views, but this will only take a couple of minutes at most.

Now if the second sheet is SMALLER than the original, you may get a warning that you can't move a view 'Off the Drawing'. What this means is that you will probably have to first drag the views toward the lower left corner of the original drawing sheet before attempting to drag the views from one Sheet to the other, and then afterwords move them around until they line-up where you want them to on the new drawing sheet.

Now once you've moved all of the views to the new sheet, just go into the Part Navigator and delete the original sheet after which you can even rename the new sheet the same name as your original sheet so that no one will ever be the wiser as to the fact that the drawing has been resized.

I know it sounds like a lot of work, but if you only have to do this once in awhile, it can save the work of starting over.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
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.

 

[uwam2ie]

... thank u John
in old Ug(v18)version we have had a UGtools program using pattern - //I haven't had since since v18 ( why?? other question). With UGTOOLS I had only to choose the new drawing size... every other things automated.
... was pretty cool. should be a nice enhancement every drawer wants to have.
thx

 

[symphony123]

John,
I am using NX 6. As it is seen in the enclosed attachment, somehow Bolt circle and bolt holes dimensions could not be captured. So still there is some re-work at this location after replacing the component.
I tried to work on this several different ways but still that dimension circled doesnt come out correctly.
could you please guide if I am missing something.
I appreciate your guidance.
Thankyou very much!!

 

[JohnRBaker]

Yes, there are still some issues with Bolt-Circles, however try this first. When you open the drawing, doubled click on the Bolt-Circle symbol as most the time it will at least partially update automatically. Granted, if there are now more holes than what was in your template, you may have to select the 'missing' holes when updating the Bolt-Circle symbol, but usually that's all that's needed to fix Bolt-Circles, particularly in NX 6.0.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
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.