NX9 Drafting-show one part drawing on another part drawing

[51Mike]

I would like to show an entire single sheet drawing of one part as an entire sheet of another part drawing,and have all of the dimensions and notes update on both drawings.

 

[Xwheelguy]

So let me guess, you have 2 different drawings of 2 different parts already completely done? Don't think you can do this, at least as easily as you'd like. At best, you're probably going to have to recreate 1 of the 2 drawings entirely if you're going to insist on having your cake and eating it too.

Let's say we have PartA dwg and PartB dwg. If it were me and PartA dwg was going to be the most difficult to recreate or take the longest, I'd save PartA dwg as a new file, add PartB as a component, add a new dwg sheet (let's call it sheet2). Place the same views on sheet2 as were on old PartB dwg, use Hide Component to hide PartA in these new views on sheet2 and then add all the dimensions, annotations, notes, etc. Some of the annotation or notes can be copy/pasted from old PartB dwg to new PartB sheet2.

I think that's about as good as it's going to get for you and I hope my blabbering makes some sense.



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

 

[51Mike]

I will try to elaborate but keep it simple. One example would be the end form of a typical automotive steel fuel tube. Every tube is different, yet the end form geometry is the same, per standard. I can make a part file of the end form geometry, use it as a component in each individual tube. Now I want to make a drawing of the end form in the component file, then use that as part of each drawing for the completed tubes. Then I would not have to re-create the dimensions, surface finishes, etc. on each drawing. i would only have to do that on the end form drawing. Ideally, when I change the end form drawing, the complete tube drawings would update. if it matters, we use separate drawing and model files here.

 

[cowski]

Open the NX help and search for "drawing booklet". I've not used it, but it looks like it may be what you are looking for.

www.nxjournaling.com

 

[Crocostimpy]

You could also make it a symbol and then add it to each drawing. It won't be updateable though if you make a revision to it.

Mike

 

[Kenja824]

Im still a little confused at what you need, so this may be waaayyyy off, but I will put this out there just in case it helps.

It sounds to me like you would want to create one standard part using sketcher and expressions. Detail it up and just do save-as to each file with changes to the expressions. If the tube length is different, a bend is in a different place, etc... changing the expressions would change the part and all drafting should update if placed on the parts correctly.

You could also create a family part out of it and let the attributes you type in a spread sheet make all the changes to the part. You could put hundreds of them on the spread sheet and just adjust the expressions in the spread sheet according to each particular tube number. This however will create a new file for each part you have in the spread sheet. No save as needed. The down fall to family parts is you need to get it right with the drafting side first because any updates to the particular files will need to be done through the master in updating parts, as all files it creates are read only. (Though I have found that there is a way around that.)