Automatic Drawing Update / Lock detail view / Dimension always well placed

[stephlouv]

Hi,

I'am in charge of designing "Master model" in my company. (Yes, that's soooo coool !)
Most of our product are using the same shape and differ by their dimensions.
So, ideal for 3D parametric modeling.

No issue with the 3D and i'am using the "Visual Editor" to have a user friendly interface to manipulate the expressions.

But the main idea, at the end, is to have less as possible 2D re working.

My model can vary from 150mm to 1200mm.
I manage to have an automatic view scale selection based on expressions using model dimensions and paper dimension, that's fine.

For detail views, i've created rectangles, in the 3D model, in sketches, around the area that need detailing and I'am using it as view boundary. Perfect.
Problem A : I didn't find the way to "lock" detail view in a specific place in the drawing.

Problem B : The dimensions.
They remains well associated to 3D model but their position is a bit caotic when my model evolve from 150mm to 1200mm (yes, that's a BIG step).
So, I've created a sketch in the sheet which contrains only points and edit the dimension's origin so they are associate with a point.
It's ok but if we have to move a dimension, we now have to move a point in the sketch .... where is the gain ..?

With all these automations, my manager is still not satisfied. :-(
And he show me how they manage that in the previous CAD system, PTC Creo.
It this soft, it's possible to create in drafting application a virtual offset line (parametric) from view line that will cary the dimension.
Dimension will be on it but it's still possible to slide it along.
Is there a way to achieve this in NX 8 ?

Thanks guys for ideas.

Stéphane

"My english is bad ? That's why i'am french."

 

[JohnRBaker]

Along those lines, we've added a new option for controlling the location of linear dimensions and annotation like notes, labels and suymbols in NX 9.0 using something call 'Margins' which are defined relative to the geometry seen in a Drawing view. As the extents of the view changes due to changes in the model size these margins are updated to maintain the same relative relationship between the location of the dimensions and the extents of the model. This is similar to what we've provided for years when creating 'Ordinate Dimensions'. There is support for both an initial and secondary margin offset controlling both the location of the first set of linear dimensions relative to a model and then the distance that the subsequent sets of dimensions placed outward from the model would be located.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[stephlouv]

Good. It's planned we will upgrade to NX9 in May/june.

I've good result in editing dimension origin, "Relative to view" but then choose "Drag" + check "Associative" and link it to a robust geometry in the view.
Then, if the view is changing (but this particular point remain), the dimension will keep his relative position to this point.

"My english is bad ? That's why i'am french."

 

[stephlouv]

Is there a way to hide/supress a view ? (other solution than editing his boundary to an empty area)

A "suppress view by expression" would be usefull for automation ;-)

"My english is bad ? That's why i'am french."

 

[stephlouv]

I hate that.

My drawing already show me discrepancies.
Was perfectly fine this morning. On only applied several time different set of expression to see how to model but more important the drawing items regenerates.
A detail view suddenly stops updating.

"View Update Report
------------------

View name: DETAIL@36
View type: Detail view
Error: No solids found to section."

No Solid ?
Impossible, the parent view is updating well.

I'll try to upload a package of ( parts + drawing + .exp files ) so you try it.


"My english is bad ? That's why i'am french."

 

[JohnRBaker]

When you say that you want to "hide/suppress a view" are you talking about simply removing it temporarily or do you really want it to 'go away' without actually deleting it?

If you wish to not see the view while looking at the Drawing yet you would like it to be there when you plot/print/export a PDF of the Drawing, you can change the style of a view to 'Reference' which will remove it visually from the Drawing sheet but it will still be there whenever you plot/print/export a PDF. This is handy in that Drawing updates are faster if most of the views are set to 'reference' and you only have fully displayed the views that you're working on.

However, if you wish to actually hide/suppress a view so that it's neither seen nor 'plotted', but yet you don't want to delete it, you could try creating a second sheet which you could be used just as a sort of 'dummy' and then in the Part Navigator you could 'Drag & Drop' those views that you wish to temporarily 'hide' to this 'dummy' sheet. And when you needed them back again, just 'Drag & Drop' them from the 'dummy' back onto your working Drawing sheet.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[stephlouv]

Here is the package. Rename top zip.
Model prt file + Drawing prt file + 3x .exp to import to the model.
You can also edit it using the Visual Editor.
Thank you

"My english is bad ? That's why i'am french."

 

[stephlouv]

There is on optional chamfer on the external edge. You put his value to zero and it's supress by expression.
But the concerning view will remain on the drawing.
My manager want it as much as possible automated ....
To me, it's stupid to develop an incredible machine as when only selecting the unwanted view and press "Delete" do the job ....
But I have to show him I tried to find a solution.

Next problems are with the section F-F
To me it's not a big deal to manually move the arrow closer to the solid and rotate the section view F-F so it is horizontal.
But again, the boss want a "one clic automatic drawing". I don't think it will be possible.

"My english is bad ? That's why i'am french."

 

[JohnRBaker]

If you're getting those sorts of errors, you're probably better off contacting GTAC and having them look at your Drawings.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.