How can I set the drafting application for small format drawings? (Siemens NX) 2

[5H4D0W]

I am trying to generate some documents (pdf) from my drawing sheets in NX.

I want to use primarily A4 and A3 size sheets. ISO / NS Standard.

Firstly, the generated dimensions, symbols, and annotations, are oversized. Well, the 3.5 size of the dimension text is actually within ISO standard specs, but would be preferable at 2,5. Annotations such as view labels, SCALE, etc. are all too big. I also tried adding a point to the model to signify the center of gravity, and noticed that this too comes up too big. Sketch points made in the drafting application have the same symptom.

Secondly, when exporting pdf-documents, the lines of the drawing become oversized. So much that it hides several features, such as threads (see attachments). The only way around this, is creating a pdf though the print function, which allows me to scale the lines in the drawing by a given factor. In my example, a factor of 0.5 gives good results. (Annotations/text/dimension/symbols still a problem)

Now, my theory is that these issues arise because the standard settings of the drafting application is intended for larger drawings. These line thicknesses and font sizes work better on A0 documents. I have seen engineers make their document A0, and then print it as an A3. This isn’t really going to help, because it ruins the given scale of the drawing, effectively pushing the problem further down the line. I actually have Technician/machinist friends who have complained about improper scaling on NX-based drawings (not mine). Is this a “global” phenomenon?

In conclusion, I want to know if the drafting application has been set to large formats, can I change it, or do I literally have to create a whole new ISO-based standard in the Customer Defaults? (I have tried this, but it doesn’t give me the opportunity to change all widths. I also do not find controls for whatever is upscaling the widths in the export pdf function. There are additional elements of the drafting environment that I wish to change, that either are not present as options in the customer defaults / drafting standards, or are simply too difficult to find due to the inherent complexity of it all).

Any help on this would be greatly appreciated.

Attachments [Note: some text in Norwegian, Please ignore]:
[URL unfurl="true"]https://files.engineering.com/getfile.aspx?folder=f557fc40-0968-44c8-8a5e-2ba67f790d77&file=test17_(via_print).pdf[/url]
[link

https://files.engineering.com/getfi...972c8c314100&file=test18_(via_export_pdf).pdf

]

https://files.engineering.com/getfi...972c8c314100&file=test18_(via_export_pdf).pdf

[/url]

 

[NutAce]

Don't know if there is some kind of functionality for this.
You could make changes in your Drafting templates. Change the linewidths and text sizes on your A4 and A3 templates. These will be stored on part level.
In your drafting preferences you then need to tell NX to take the settings from the templates, rather than from the defaults file.

Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2

Building new PLM environment from Scratch using NX11 / TC11

 

[5H4D0W]

Thank you for your reply.

I have tried doing what you said. It works to some extent.

Still cant access certain options so I would advise Siemens to take a look at this problem.

What I do now is adjust symbol/text/number height by prefs, then scale down all line thicknesses through the print function.

 

[Toost]

This is a multi-setting issue.
The width is more complex than one might expect...
Each model/ body has a "width" defined, in old versions NX, Pre NX8.5, NX had 3 widths, thin , medium and thick.
The actual thickness in mm wasn't defined until plotted or maybe printed. these widths did not have a width value assigned.
( The logic of that was back in time when one physically placed a pen in a specific slot in the plotter. The pen had the actual thicknesses "0.18, 0.35mm, 0.5 mm etc " and "thin, medium, thick was mapped to the slot-s.)

NX 8.5(?) "widened the palette" to 9(?) possible width settings, each with a width value assigned.
So if you have old files you might see thicknesses like "medium" and in newer files you might see values like "0.50 mm"
There is a conversion mapping you can control, "thin== y.yy mm ; medium == x.xx mm; thick == z.zz mm "

When this model is displayed in a view on drawing, the preferences for the view MIGHT change the width into a completely different value.
"Visible lines width =0.25mm" but it can also be "visible lines width = original" ( = no change)

Then, several export options has their own settings for the value of the width. Note that "File -Print" "File-Plot" and "File-export- Pdf" all have their own settings.

All these can be set in the Customer Defaults.

Due to the complexity of the above, it is quite common that companies doesn't have the ideal settings as default...

Regards,
Tomas

 

[5H4D0W]

Hello Tomas!

Thank you for your reply on the matter. I am aware of the legacy lineweight situation, but in my case I am dealing with newer drawings. (Parts made in NX 12.0).

I have tried to edit the customer defaults, but there seems to be a multitude of menu segments devoted to lineweights and I don't think I have found the one that keeps overriding the others.

I think Siemens should address the complexity issue to make the settings more comprehensive. The current user-interface is unbelievably messy.

Regards,
Ole