Cancel
Showing results for 
Search instead for 
Did you mean: 

Constraining to the origin in a sketch

Valued Contributor
Valued Contributor

I'm new to NX, and I've noticed there are two coordinate systems available when locating or constraining geometry or dimensions relative to the origin (or X, Y axes for that matter) - the Sketch and Datum.  Is it considered better practice to use one vs the other?  I'm been using the Sketch CSYS, thinking that if I copy or move the sketch later the sketch CSYS will come with it and constraints made to that will stay intact.  But maybe I'm mistaken, so I thought it worth asking here before creating a bunch of sketches based on that assumption.  Also, if you don't use QuickPick, what is the default selection?  Thanks!

 

OriginQP.png

 

 

10 REPLIES

Re: Constraining to the origin in a sketch

Siemens Phenom Siemens Phenom
Siemens Phenom

When new sketch is created, seperate datum csys is created as there is option 'Create Intermediate Datum CSYS' remain selected under the settings of create sketch window. By selecting the sketch > RMB > Make Datums External, It will show the new csys in part navigator above the sketch.

 

If you do not want intemediate sketch to be created, simply you can deselect the option in create sketch window or you can set it under customer defaults (File > Utilities > Customer Defaults > Sketch > General > Session Settings tab > Deselect option 'Create Intermediate Datum CSYS through Create Sketch Dialog')

 

Not creating sketch with intermediate datum csys and use of absolute csys, Sketch will consume the aboslute csys which you need to make it external if you want to use its planes,axes as reference later. By doing so if absolute csys is deleted, It will delete all the features for which it was referenced. Create a sketch by using plane of absolute csys with intermediate csys option turned on. Delete the absolute csys it will show notification that features will get affected but sketch remains in part navigator with no reference and it will show a alert symbol for sketch. You can use reattach sketch then. It will depend upon you how to use it. Smiley Happy

 

 

Re: Constraining to the origin in a sketch

Siemens Phenom Siemens Phenom
Siemens Phenom

Hi,

 

When sketching try to make internal references as much as possible.

 

NX provides a sketch origin and two axes for this. Using these makes it easier to reattach the sketch later on. When reattaching you cannot reparent constraints and dimensions to external objects in an easy way. So the more you have internal, the better.

With the intermediate datum coordinate system the sketch will will also update in a more predictable way when the context changes due to a model edit.

 

Please do not change settings related to internal datum coordinate systems or associative origin for sketcher. Use the internal datum coordinate system. It is there for the reason described above. It allows the sketch to have an associative origin so curves to not wander off into deep space during modification of the part.

 

Also note... we removed the ability to turn off intermediate datum CSYS for sketches in NX 11. The default settings we defined in NX 7.5 are the way forward. 

 

Regards, **bleep**

 

 

Re: Constraining to the origin in a sketch

Valued Contributor
Valued Contributor
Thanks for the replies.

To clarify, is it correct that a sketch is normally attached to a Datum CSYS (Datum Coordinate System (0) in the example above )? If so, what is the advantage of that compared to having it attached to the Absolute CSYS?

Re: Constraining to the origin in a sketch

Siemens Phenom Siemens Phenom
Siemens Phenom

When you create a sketch and on the create sketch dialog just press OK then the sketch is not attached to anything (in NX 11). It is fixed in space but you can reattach it. When you reattach you will see the inputs for the plane, direction and origin set to fixed.

 

If you select a plane of the datum CSYS in the part then the inputs will all be attached to that datum CSYS. When you move the CSYS the sketch will go with it.

 

Regards, **bleep**

Re: Constraining to the origin in a sketch

Valued Contributor
Valued Contributor

Thanks again.  The more I look at this, the more I realize I am not fully grasping something.  So let me back up.

 

When I first open the modeling template (model1.prt), NX creates a default datum CSYS (Datum Coordinate System (0))

datumCSYS0.png

 

If I then select Sketch (in Direct Sketch group) a Sketch dialog opens.  The default settings (at the bottom) are set to create an Intermediate Datum CSYS with associative origin when the sketch plane is selected.  

createSketchDialog.png

So if I'm understanding this correctly, there are 3 coordinate systems involved here:

1. Datum Coordinate System (0)

2. Intermediate Datum CSYS

3. Sketch

 

Is that right?

 

If I then select, say, the XY plane of Datum Coordinate System (0), does NX create an Intermediate Datum CSYS coincident, and aligned with, Datum CSYS (0)?  And does the Sketch CS then get placed on, and referenced to, the Intermediate CSYS?

 

 

 

 

 

Re: Constraining to the origin in a sketch

Siemens Phenom Siemens Phenom
Siemens Phenom

Were are almost there...

 

There are two features:

1. The datum CSYS feature (0)

2. The Sketch (1)

 

The sketch contains a datum CSYS, but you only see that represented as the origin and the H and V axes.

When you reattach the sketch you are actually editing a datum CSYS. From NX 11 is is very clear because the UI is more aligned.

With internal datum CSYS turned on the sketch is always on the internal datum CSYS.

 

Now when you create a sketch and you select a plane from datum CSYS (0) feature, then the internal datum CSYS (and thus the sketch) is referring to the datum CSYS feature (0).

 

I hope this helps... In NX 11 we made it easier by removing the options that you should not use. 

 

Regards, **bleep**

 

PS. One more thing on create and reattach sketch, we are writing the book on it anyway. Avoid using a vertical reference. There is a known problem with it in NX 10 and before. Using it can lead to confusing situation where horizontal and vertical sometimes seem to be missed up. 

Re: Constraining to the origin in a sketch

Valued Contributor
Valued Contributor

Thanks for the additional explanation.  This is starting to come together now.

 

To get a better grasp on this, I did some simple tests. I first created a sketch without an intermediate (internal) datum CSYS, so it attached to datum CSYS(0).  The sketch made datum CSYS(0) internal (consumed it?).  I then made it external and deleted it.  When I did that, the sketch disappeared as well!  I assume any associated features would have gone with it (as Ganesh alluded to in his reply).  So I guess that illustrates the risk of not using an internal datum!

 

I tried this again, but this time used the intermediate datum.  When I deleted datum CSYS(0) the sketch remained intact.

 

What puzzles me about this though, is if the sketch has it own "sketch CSYS"  (apart from the Intermediate or CSYS(0) datums) why does it disappear when those are removed?  At first I was thinking it was because there is nothing to tell it where it's located in the model space, but that would be true in the second case also, since without datum CSYS(0), how would the internal datum know where it is?  So there must be something about the sketch CSYS that makes is different from a normal datum (maybe some information it's missing that won't allow it to "float" a sketch).  Is there?

 

Thanks for any further insight into this.  I think I'm almost there. Smiley Happy

 

Pat

Re: Constraining to the origin in a sketch

Genius
Genius

Hello,

 

you have to split the two features Datum CSYS and Sketch. A sketch can't exist without a basic object. When you remove the parent from the sketch, the feature runs into an error.

 

The Datum CSYS is special, because when you remove the parent of the Datum CSYS the feature get into a fixed state.

 

And that's the difference between the two states. When you create a sketch direct on a D-CSYS and you delete the CSYS, the sketch has no parent and run into an error. When you have an internal CSYS, this CSYS get in fixed state and is still the parent of the sketch.

 

Regards André

Re: Constraining to the origin in a sketch

Valued Contributor
Valued Contributor

The Datum CSYS is special, because when you remove the parent of the Datum CSYS the feature get into a fixed state.

 

 


Thanks for the response.  By "fixed state" do you mean a Datum CSYS with a deleted parent gets assigned it's absolute position (w.r.t. the Absolute CSYS)?