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round holes showing up as squares 1
- Thread starter mco
- Start date
have you checked if Lightweight loading is used.
An other reason could be visualisation settings.
I have had the problem weeks ago. Preferences -> Visualization
the facetting card, Partsetting, shaded views tolerance, use standard.+ regenerate view -> View -> operation-> regenerate view
regards
An other reason could be visualisation settings.
I have had the problem weeks ago. Preferences -> Visualization
the facetting card, Partsetting, shaded views tolerance, use standard.+ regenerate view -> View -> operation-> regenerate view
regards
JohnRBaker
Mechanical
If the holes are in a Component of an Assembly it could be that you are using Lightweight Representations (which is a good thing from a graphics performance point of view). If it's a single piece part then perhaps you have your display tolerance set too high (or too low, depending on how you think of it). Try this, zoom-up on your model and then perform a...
View -> Layout -> Display Update
...and if this improves your display (circles no long look like squares) then you may need to change your display tolerance by going to...
Prefernces -> Visualization -> Faceting
...and in the section of the dialog titled 'Part Settings' change the Shaded View 'Tolerance' to something like 'Fine' or 'Extra Fine'. Note that this will only change the display tolerance of this single part file. If you wish top change your systems default, you will need to go to...
Customer Defaults -> Gateway -> Visualization -> Facetting
...and make a global change, but remember this will only effect new files created which did NOT use a template file. If you use a template file, you will need to Open the template file, make the first change above and save it.
However I must warn you that setting the display tolerance to high will have a negative impact on display performance. You need to trust in the idea that despite what you might see on the screen that the holes are actually ROUND and that having the 'luxury' of seeing them as perfect circles comes with a 'price'. I would recommend that you use the Update Display when you wish to assure yourself that you're getting what you expected and just trust the system the rest of the time to be doing what you expect it to be doing.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
To an Engineer, the glass is twice as big as it needs to be.
View -> Layout -> Display Update
...and if this improves your display (circles no long look like squares) then you may need to change your display tolerance by going to...
Prefernces -> Visualization -> Faceting
...and in the section of the dialog titled 'Part Settings' change the Shaded View 'Tolerance' to something like 'Fine' or 'Extra Fine'. Note that this will only change the display tolerance of this single part file. If you wish top change your systems default, you will need to go to...
Customer Defaults -> Gateway -> Visualization -> Facetting
...and make a global change, but remember this will only effect new files created which did NOT use a template file. If you use a template file, you will need to Open the template file, make the first change above and save it.
However I must warn you that setting the display tolerance to high will have a negative impact on display performance. You need to trust in the idea that despite what you might see on the screen that the holes are actually ROUND and that having the 'luxury' of seeing them as perfect circles comes with a 'price'. I would recommend that you use the Update Display when you wish to assure yourself that you're getting what you expected and just trust the system the rest of the time to be doing what you expect it to be doing.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
To an Engineer, the glass is twice as big as it needs to be.
- Thread starter
- #5
Thanks, this helped. I had already changed my settings from lightweight to show exact, but the changes didn't immediately take effect. I am now seeing the parts as they should be.
Right now, I am just comparing two parts, so performance isn't an issue. I agree, John, that there is a price to pay performance wise. Thanks for providing the path to the solution.
Right now, I am just comparing two parts, so performance isn't an issue. I agree, John, that there is a price to pay performance wise. Thanks for providing the path to the solution.
While on the subject:
We just received a part from our subcontractor where the slotted holes are cut out as 8-corner polygons. This was caused by creating and exporting the drawing while using lightweight. (export via file>export>2D exchange)
On the PDF we couldn't see the polygons, but they were visible on the dwg's and dxf's (which, unfortunately, we didn't check before we sent over the files)
Is this supposed to happen? Is there a way to prevent this without giving up lightweight?
NX7.5.4.4 (+teamcenter 8)
We just received a part from our subcontractor where the slotted holes are cut out as 8-corner polygons. This was caused by creating and exporting the drawing while using lightweight. (export via file>export>2D exchange)
On the PDF we couldn't see the polygons, but they were visible on the dwg's and dxf's (which, unfortunately, we didn't check before we sent over the files)
Is this supposed to happen? Is there a way to prevent this without giving up lightweight?
NX7.5.4.4 (+teamcenter 8)
JohnRBaker
Mechanical
When you open a drawing of either an Assembly or a single Component (when working in Master Model mode) even if you loaded the assembly using Lightweight representations, the drawing will automatically ONLY utilize the precise models. Now on the other hand, if the user explicitly asked that the drawing views be created using faceted models, then all bets are off as to what the final results are going to look like. Note that I'm only taking about NX 7.5 here since before the current release the user was responsible for making sure that the drawing was getting the proper representations, but starting with NX 7.5, if you followed our out-of-the-box setup and you used lightweight for your assemblies, your drawings would automatically to created as they needed to be to look and behave as one would expect a drawing to behave. However, if you're dealing with a legacy drawings then you will need to run them through the refile utility to get everything properly saved and set-up. Simply opening the assembly and thinking that the on-the-fly update will take care of everything if you then save the models and drawings will not always catch everything. Only if you use refile on ALL your part models, including library parts (family table members), will you be sure of catching everything.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
To an Engineer, the glass is twice as big as it needs to be.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
To an Engineer, the glass is twice as big as it needs to be.
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1
- #9
cwdunwoody
Mechanical
Well its Windows 7 Proffesional, version 6.1. It has 2GB of ram. NX 6.0.5.3. However, there are many other computers in the office running the same version of nx and the same hardware without any problems but I think many of them are running xp. I do think though there are some machines that have been running windows 7 successfully. Here's a pict of the problem it's having.
JohnRBaker
Mechanical
THAT'S a totally different problem. And while it might very well be the graphics driver, before you go and mess with anything like that give this a try: Go to...
View -> Camera -> Edit...
...and when the dialog comes-up, go down to the section labeled 'Clipping', push the 'Fit Planes to Extents' button and then hit OK. Did this 'clean-up' your display? If not, then it's time to look more closely at the display drivers that you're using.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
To an Engineer, the glass is twice as big as it needs to be.
View -> Camera -> Edit...
...and when the dialog comes-up, go down to the section labeled 'Clipping', push the 'Fit Planes to Extents' button and then hit OK. Did this 'clean-up' your display? If not, then it's time to look more closely at the display drivers that you're using.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
To an Engineer, the glass is twice as big as it needs to be.
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