How to adjust my UCS

[Adrian2]

Dear Folks;

While making the drawing files for a number of in-context parts in a SW2003 assembly, I found that the parts were not in a convenient view orientation for dropping into a drawing border.

To fix this I had to go back into the part files and create some "hidden" feature on the face of the part to allow me to drop the part onto the sheet in the orientation I wanted. I cannot imagine that this is the right way to go about reorientating views so I wondered if anyone could help explain the proper way.

In Mechanical Desktop I could adjust the UCS of the part to compensate for this problem but I have found no way doing this in the SW help files. Perhaps I am just searching using the wrong terminology.

As always I am forever grateful for the help I receive from the experts here !

Regards

Adrian D.

 

[Theophilus]

If you're attempting to drop your part into a drawing (instant three views), you will need to redefine your "Front" view in your part.

I haven't done this lately, but the way I did it in past versions was to reset my Front view to the orientation I wanted. Doing this may reset a few other things, so make sure you really want to make this change first.

In your part view, orient the part according to the front view of your three-view drawing. Hit the space bar to bring up your orientation control. Select the front view listed and hit the Update View button on the orientation control window. This should reset your view so you can drag your part into a drawing document and get three views.

An alternative to this method is to orient your part the way you want it and then place each view in the drawing individually. Then align each view to your primary view. This method is more labor-intensive, but does not require you to reset your primary view (and therefore all your other views).

I hope that helps.


Jeff Mowry
DesignHaus Industrial Design

http://www.designhaus-i-d.com

 

[Adrian2]

Dear Jeff;

Thanks for your answer but I know how to manipulate views and select the ones I want to drop into my drawing.

If, for example, you have a circular plate with 4 holes on a bolt circle, and you want the front view of the part to have the top hole in the 12 noon position on the drawing sheet. But the front view in the part has the hole at the 1 o'clock position. How do you get the hole to the 12 noon position on your drawing sheet without altering the sketch in the part and affecting the in-context geometry ?.

Best Regards

Adrian

 

[dsi]

Select the drawing view and hit the Rotate View button(near the zoom and pan buttons). This will pop up a menu for selecting the rotation angle. DimensionalSolutions@Core.com
While I welcome e-mail messages, please post all thread activity in these forums for the benefit of all members.

 

[Adrian2]

Dear dsi;

OK, tried your suggestion, it turns out that in order to get my view into the right position I have to rotate it 2.32 degrees. The view rotated and displayed properly. Only thing is, all the dimensions now display rotated at 2.32 degrees. Its also next to impossible to sketch a section line that passes through the supposedly aligned holes on the bolt circle.

There are also alignment commands, but they only work when you have another drawing view to align to. I am working on the primary view. So far the onlt thing that I that works is to sketch a surface onto the part rotated 2.32 degrees from centerline. Then I take a view "normal-to" that surface. After everything displays OK I go back and hide or suppress the surface feature.

Thank you anyway for trying, the rotate view procedure is sure to be useful another time for another task

Regards

Adrian

 

[Theophilus]

Adrian2,

Double-check the instructions from my first post about updating your standard views. This works fine. If you orient your part to where it needs to be for your front view, you can permanently change the representative front view to match your part's orientation in your window.

In your case, orient your part so you have the 2.32 degrees (or so your hole is at 12:00 position). If this is the front view you want, hit the space bar to bring up your orientation control and hit the "update standard views" button. I just tried it in SW 2003 and it still works. Then, drag your part into a new drawing and it will lay out all three standard views perfectly.


Jeff Mowry
DesignHaus Industrial Design

http://www.designhaus-i-d.com

 

[TheTick]

try using "Insert-->Drawing View-->relative to Model"

This allows you to use model faces to orient your drawing views.

Caution: if the view is not "square" to the root datums, the view defaults to isometric dimensioning. Be sure to change the view properties to projected dimensioning. If you change the dimensioning mode, you will lose all of the dimensions in that view. Gravity is a harsh mistress.

 

[SnowCrash]

To get a view exactly normal to a feature you can create a plane in line with the feature, select the plane, view normal to that one, rotate it 90 deg and create a new view based on that or redefine all your views based on that requirement. Insert that view into your drawing and derive[project] the rest from there. This even works if your angles are irrational.

Crashj 'who is not really all that irrational' Johnson

 

[dhinners]

There is another way to 'align' your views. The only requirement is a feature with a straight edge that you can use to specify your vertical or horizontal. Say that as mentioned you had a round plate with a hole pattern that was not orthogonal to your datum planes. First make a configuration of your part with a feature that is aligned to your holes. Then insert the primary view as the view that shows the holes as circles. Select an edge that you want to see as horizontal (MUST SELECT FIRST) then use

Tools > Align Drawing View > Horizontal Edge

Your view will rotate to the exact angle required. Any dependent views you have already created will also update. However, I believe you will have to recreate any dimensions that already exist. Also, as far as I know you cannot insert ordinate dims correctly.

The last step would be to change the referenced configuration to one without the alignment feature.

p.s. I am verifying these steps using SWX 2001-plus - I do not have access to 2003 right now.

 

[dhinners]

By the way - if your features are not aligned to the datums only because you built them in-context, there is a another fix you could try. Usually parts made exclusively in-context are mated into your assembly with an in-place mate. I like to delete that mate, then remate the part using its datum planes in a way that makes sense relative to the expected part features. Usually it pays to take this step before making any features to avoid lots of red assembly flags. Even so, as long as your geometry is totally defined in-context you will see it update when you redo the mates.

 

[JNR]

Adding to dhinners' comments. Once you have your custom aligned view created - name it something standard and useful. Drawing Templates (or Formats, or whatever the current buzz word is) can now have predefined sets of views on them - not just drag-n-drop top/front/right. So if this is a common occurance you should be able to really automate it. Even if the first "front" view is custom and is a bit different from part to part, you could probably name it with a single standardized name and have the other views pre-defined by projection or aux-views from it. I do hardly any "drafting" but whenever I meet a new CAD system or a new Revision I read the manual from cover to cover, so it's floating round the back of the mind somewhere. So you will need to look into this, check that it works and refine it.