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Snapping to closest iso view when placing a view in drafting
- Thread starter chopper75
- Start date
JohnRBaker
Mechanical
When you use the 'Add Base View...' function you will note an option in the 'Model View' section of the dialog titled 'Orient View Tool'. Select it and small secondary 'window' will open showing your model. Using either your Spaceball or the normal mouse gestures you can rotate the view around until you get what you've looking for. Once you have what you want, simply hit the OK button in the 'Oreint View Tool' dialog and it will capture that view orientation and then you simply finish placing the view.
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.
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.
Not to my knowledge. ( no simple and quick methods that is.)
But, what is a "correct iso view" ? I do know the definition, but does it matter ?
In my opinion, the purpose for a drawing is to transfer information between the designer and the reader, and the faster and simpler that can be done, the better. - if the view shows what you desire to present , that is the view to place.
The not so quick and simple way to create an iso view is to turn of the display of the drawing , use the F8 to snap the view such that the left side of the view to come is flat parallel to the screen.
Then View - rotate, select Y and rotate -45 degrees. ( Y in this case is Screen-Y, not WCS-Y), then select X and rotate +~35.2644 degrees.
OK the dialog , View - Operation - Save As, enter a name for the view, display the drawing again and finally place the saved view.
Regards,
Tomas
But, what is a "correct iso view" ? I do know the definition, but does it matter ?
In my opinion, the purpose for a drawing is to transfer information between the designer and the reader, and the faster and simpler that can be done, the better. - if the view shows what you desire to present , that is the view to place.
The not so quick and simple way to create an iso view is to turn of the display of the drawing , use the F8 to snap the view such that the left side of the view to come is flat parallel to the screen.
Then View - rotate, select Y and rotate -45 degrees. ( Y in this case is Screen-Y, not WCS-Y), then select X and rotate +~35.2644 degrees.
OK the dialog , View - Operation - Save As, enter a name for the view, display the drawing again and finally place the saved view.
Regards,
Tomas
- Thread starter
- #4
John, thanks a lot for your help. I have been doing exactly what you are saying. The thing that I'd like to do is sort of "snap" to the closest iso view. I want my vertical edges to be trully vertical. Not approximately vertical as it turns out when I do it by eye. This is again an exploded view and from my understanding I have to use the "TFR-TRI" model view to capture an exploded view?...
- Thread starter
- #5
JohnRBaker
Mechanical
I'm so sure what you mean by the 'closest iso-view' as there are an infinite number of them. However, that being said, we have a little known option which allows you to add an additional 16 predefined so-called 'Dimetric Views'. To enable these additional views, which will automatically be added to any of your existing files upon opening them, go to...
Customer Defaults -> Gateway, -> General -> Part
...and near the bottom of the page you will find an option titled 'Add Dimetric Views'. Toggle it ON, hit OK and restart NX.
Now there is a warning, once these views have been added to your part file, toggling this option OFF will NOT remove the 16 extra views. If later on you decide you don't want to see those 16 extra view names every time you open up a list of available views, you'll need to remove them manually. So I would experiment with a couple of simply files and see is this gives you something that you can work with.
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.
Customer Defaults -> Gateway, -> General -> Part
...and near the bottom of the page you will find an option titled 'Add Dimetric Views'. Toggle it ON, hit OK and restart NX.
Now there is a warning, once these views have been added to your part file, toggling this option OFF will NOT remove the 16 extra views. If later on you decide you don't want to see those 16 extra view names every time you open up a list of available views, you'll need to remove them manually. So I would experiment with a couple of simply files and see is this gives you something that you can work with.
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.
- Thread starter
- #9
John,
Thanks. I added the dimetric views and still doesn't give me what I'm looking for. Perhaps I'm stuck in what I'm used to doing in other CAD packages. I think I've found a way to get my Iso views the way I want them. It just takes a couple of steps. Sort of what Toost mentioned. I'll snap to Ortho, then tilt X and Y axes to desired amount. I basically just need my "Z" vertical. I don't care about being in a standard Iso. I just don't want my views kind of "leaning" to one side which is what I always end up with when using the orient tool.
Thanks again for your help
Thanks. I added the dimetric views and still doesn't give me what I'm looking for. Perhaps I'm stuck in what I'm used to doing in other CAD packages. I think I've found a way to get my Iso views the way I want them. It just takes a couple of steps. Sort of what Toost mentioned. I'll snap to Ortho, then tilt X and Y axes to desired amount. I basically just need my "Z" vertical. I don't care about being in a standard Iso. I just don't want my views kind of "leaning" to one side which is what I always end up with when using the orient tool.
Thanks again for your help
You could set up and save all your ISO views in your part template file, then they would all be ready to go when you need them. No need to recreate them in each part.
www.nxjournaling.com
www.nxjournaling.com
JohnRBaker
Mechanical
What version of NX are you using?
And when you say 'Z' is vertical, do you really mean that you want so-called vertical lines to appear to be pointing up with no VISUAL tilt?
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.
And when you say 'Z' is vertical, do you really mean that you want so-called vertical lines to appear to be pointing up with no VISUAL tilt?
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.
- Thread starter
- #12
JohnRBaker
Mechanical
But if 'Z' is truly UP or 'vertical', then it would NOT be an isometric view.
Since you're using NX 7.5 try this. While in Modeling, open your part file and orient the display to one of the orthographic views (Top, Front, Right, etc.) so that what you want to remain vertical or 'UP' is actually pointing UP.
Now look down at the bottom-left corner of your screen and you will see what looks like a small Red/Green/Blue CSYS. One of the axis will be pointing UP (or DOWN depending on which view you picked) and one should be pointing either to the left or to the right (the 3rd axis will be pointing directly toward or away from you but you can ignore that one for now).
One word of caution here, this is one of those times when IF you have a Spaceball attached to your system DON'T TOUCH IT! Do everything with your mouse.
Now select using your cursor the axis which is horizontal, pointing either to the left or the right, and you will see a small entry window pop-up where you can type in a desired rotation angle, or, while holding-down on the MIDDLE mouse button, you cam move the cursor up or down and the model will rotate about that selected axis. So either enter an angular value or move the mouse until you get at least the starting of the orientation that you're looking for. Once you think you're close stop and select whichever was the axis which was initially vertical (going UP or DOWN). Again, either by typing in a value or now using the cursor, while holding-down the middle mouse button, moving to the right or to the left, rotate the view until you get your desired 'isometric' orientation.
Now go to the Part Navigator, expand the item labeled 'Model Views', highlight the item labeled 'Model Views', press MB3 and select the 'Add View' option and you will see a new view added to the list which if you slowly double-click it you will be given the chance to rename it to whatever you want to name it, say ISO-1 or something.
Now when you go to add a view to your drawing, when you select the 'Add Base View' option and the dialog comes-up, in the Model View section of the dialog when you expand the list of available views you will see the name of view which you just created. Select it and place it on your drawing.
Now this may sound a bit convoluted but with a bit of practice you can define any sort of view that you wish, save it so that it can be accessed in places like a drawing, and you should be good to go.
Anyway, give it shot and let us know what you think.
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.
Since you're using NX 7.5 try this. While in Modeling, open your part file and orient the display to one of the orthographic views (Top, Front, Right, etc.) so that what you want to remain vertical or 'UP' is actually pointing UP.
Now look down at the bottom-left corner of your screen and you will see what looks like a small Red/Green/Blue CSYS. One of the axis will be pointing UP (or DOWN depending on which view you picked) and one should be pointing either to the left or to the right (the 3rd axis will be pointing directly toward or away from you but you can ignore that one for now).
One word of caution here, this is one of those times when IF you have a Spaceball attached to your system DON'T TOUCH IT! Do everything with your mouse.
Now select using your cursor the axis which is horizontal, pointing either to the left or the right, and you will see a small entry window pop-up where you can type in a desired rotation angle, or, while holding-down on the MIDDLE mouse button, you cam move the cursor up or down and the model will rotate about that selected axis. So either enter an angular value or move the mouse until you get at least the starting of the orientation that you're looking for. Once you think you're close stop and select whichever was the axis which was initially vertical (going UP or DOWN). Again, either by typing in a value or now using the cursor, while holding-down the middle mouse button, moving to the right or to the left, rotate the view until you get your desired 'isometric' orientation.
Now go to the Part Navigator, expand the item labeled 'Model Views', highlight the item labeled 'Model Views', press MB3 and select the 'Add View' option and you will see a new view added to the list which if you slowly double-click it you will be given the chance to rename it to whatever you want to name it, say ISO-1 or something.
Now when you go to add a view to your drawing, when you select the 'Add Base View' option and the dialog comes-up, in the Model View section of the dialog when you expand the list of available views you will see the name of view which you just created. Select it and place it on your drawing.
Now this may sound a bit convoluted but with a bit of practice you can define any sort of view that you wish, save it so that it can be accessed in places like a drawing, and you should be good to go.
Anyway, give it shot and let us know what you think.
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.
JohnRBaker
Mechanical
One thing I forgot to mention: Between selecting the arrows on the small colorful CSYS in the corner, always hit the 'Esc' button to close the small entry window. Also once you get to where you almost like the view you have but you want to make a slight adjustment which will NOT mess-up the visually 'vertical' orientation of your view while in modeling, simply move your cursor to the far left or right side of the screen and while you have the cursor as closse to the edge of the NX display window as possible, hold-down the middle-mouse button and move your sursor up or down and you will onlybe rotating the model about horizontal axis of the screen meaning the 'vertical' lines will remain vertical (at least visually). But if you wish to rotate about the vertical axis just select whatever axis of that small colorful CSYS in the corner is point up and then using your cursor you can rotate about the so-called vertical orientation of yoru display. Just remember that once you move the display you will need to go back to the Part Navigator and select the view on the list of Model Views, press MB3 and select the 'Save' option so that the new orientation is saved.
And if you've already placed you view on the Drawing you can still do something like this by selecting the Drawing View, pressing MB3 and selecting 'Edit...'. When the Edit view Dialog comes up, in the Model View section of the dialog, select the 'Orient View Tool' and the you can manipulate THAT view in the little preview window (which can be scaled larger by dragging one of the corners) using the same mouse cursor techniques which I described above only now doing this inside the smaller preview window. And once you get it the way you want it, just hit the OK button on the 'Orient View Tool' dialog and the drawing view will be updated.
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.
And if you've already placed you view on the Drawing you can still do something like this by selecting the Drawing View, pressing MB3 and selecting 'Edit...'. When the Edit view Dialog comes up, in the Model View section of the dialog, select the 'Orient View Tool' and the you can manipulate THAT view in the little preview window (which can be scaled larger by dragging one of the corners) using the same mouse cursor techniques which I described above only now doing this inside the smaller preview window. And once you get it the way you want it, just hit the OK button on the 'Orient View Tool' dialog and the drawing view will be updated.
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.
- Thread starter
- #15
- Thread starter
- #16
Another little trick , if all you need is to rotate the view which is already ON the drawing.
Double click the view border, select the tab "orientation", this tab actually allows one to rotate ( all directions) a placed view, but one must use the options there. ( spaceball and such is "off")
The button "Define X Direction" can be used to select something that will become ( the view rotated about the "paper normal")
horisontal on the sheet. In your case you desire "vertical", so try to pick or define ( two points ?) something which is perpendicular to Y. Press Apply to see result. I created/ sketched a helper line constrained perpendicular to the verticals, then deleted the helper line. the view rotation isn't associative so it works.
Double click the view border, select the tab "orientation", this tab actually allows one to rotate ( all directions) a placed view, but one must use the options there. ( spaceball and such is "off")
The button "Define X Direction" can be used to select something that will become ( the view rotated about the "paper normal")
horisontal on the sheet. In your case you desire "vertical", so try to pick or define ( two points ?) something which is perpendicular to Y. Press Apply to see result. I created/ sketched a helper line constrained perpendicular to the verticals, then deleted the helper line. the view rotation isn't associative so it works.
You can have the 'nearest iso view' in 1 button press - set a system environment variable UGII_FKEY_DYNAMICS with the value of 1 and this turns F1, F2, F3 and F4 into Pan, Zoom, 3D Rotate and 'Snap to nearest ortho or iso view'. Using F4 with the Orient View button in the Base View command is defintiely your friend.
Note that this extra functionality only occurs when your mouse is over the graphics window - they function as normal when placed over toolbars, Part Navigator window etc.
HTH,
Jon
JHTH
NX 7.5.5 + TC 8.3.2.2
Note that this extra functionality only occurs when your mouse is over the graphics window - they function as normal when placed over toolbars, Part Navigator window etc.
HTH,
Jon
JHTH
NX 7.5.5 + TC 8.3.2.2
JohnRBaker
Mechanical
Just so everyone understands, this use of the F1 thru F4 keys to manipulate the display was done to accommodate people transitioning from I-deas to NX since many of them were unfamiliar with using either a 'Spaceball' or mouse-gesture initiated display control. This option enabled for them the same user-interaction that they had had with I-deas when it came to display control.
The reason that this was NOT adopted as the 'standard' behavior with NX was that the vast majority of UG users were already well versed in the use of either 'Spaceballs' or using mouse-gesture initiated display control and besides, the 'Fx' keys were already being used for other things and while it is true that where your cursor is positioned does effect how these first four function keys were interpreted, it was still seen by many people (true, these were mostly legacy UG users) as being a bit klunky when something like a 'Spaceball' almost completely negated the advantages of having function key initiated display control in the first place. And with the price of 'Spaceballs' coming down and with virtually every system already coming with a 3-button mouse, it was decided to offer this alternative behavior as only an option.
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.
The reason that this was NOT adopted as the 'standard' behavior with NX was that the vast majority of UG users were already well versed in the use of either 'Spaceballs' or using mouse-gesture initiated display control and besides, the 'Fx' keys were already being used for other things and while it is true that where your cursor is positioned does effect how these first four function keys were interpreted, it was still seen by many people (true, these were mostly legacy UG users) as being a bit klunky when something like a 'Spaceball' almost completely negated the advantages of having function key initiated display control in the first place. And with the price of 'Spaceballs' coming down and with virtually every system already coming with a 3-button mouse, it was decided to offer this alternative behavior as only an option.
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.
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