Working With Datum Targets

[KENAT]

I'm working on a drawing & model of a casting and the subsequent machining step. Only some of these points are explicitly tied to physical geometry, the others are just a theoretical point on a surface.

Any ideas on how best to tie these to apply these? I'm having trouble tieing them to a drawing view and getting them to move with it. Should I just make the dimension driving, or is there another way. I'm loathed to put sketches of points in unless I really have to.

Thanks, a slightly rusty on SE KENAT.

KENAT,

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[donyoung]

Ken,

I would suggest to select the view, RMB -> properties
then select 'DrawInView'. When put there they will
always move with the worksheet's view. You can put some
constraints to them and dimensions as well. For the
dimensions activate a separate layer so that you can
hide it and thus they will not be visible in the view.

dy

 

[KENAT]

Thanks Don, that's kind of what I'd started to do but of course being in draw in view & related to the view I can't make those dimensions driven, or am I missing something? I can obviously locate them by drawing in some geometry and attaching them to it & put that on a layer as you say but I'm concerned if someone else comes to work on it later they won't have a clue what's going on.

I was thinking of creating a sketch in the model of very small X to locate them to, sound reasonable? I was going to put actual datum targets in the sketch but couldn't get dimensions to them to be driven.

KENAT,

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[donyoung]

Ken,

hmm, maybe I didn't get the picture. When in 'Draw in view' and
put a datum target (with that function) and dimension the
datum point to one of the edges of the model the dimension
is driven. When the edge I've dimensioned to moves because
of a change to the model the dimension will change.
When the datum target is attached to an edge or the like
it will move with that edge.
Placing a 'hand crafted' datum target and dimension it then
you have the choice of a driving or driven one

dy

 

[KENAT]

I said the wrong thing, I meant I can't make those dimension driving.

Thanks for what you've put though, it kind of confirms I'm not missing something simple.

Ken

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[beachcomber]

Drawing views have a layer called Auto-hide (in Draw-in-view).
If you put anything on this layer it will not show when you go back to the working sheet.
It's common pratice to put some construction in a view - like lines to show the intersction of 2 edges, or offsetting edges to indicate an extent of a surface preparation.
I'm not fully clear on what you want to show - could you provide an example picture?

bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.

 

[Raaden]

Couldn't you just draw a line in the view, attach the datum target to the end point of the line and then drive the line with a dimension? (line and dimension goes into auto-hide layer)

 

[KENAT]

Beach the part I'm working on is IP sensitive, but simplistically imagine you've got a cast part with some relatively complex surfaces. I want to put datum targets (using that function) at points on those surfaces that don't have explicit geometry to associate them to, instead they are a defined dimension from other datum points.

Raaden, unless I'm mistaken Dimensions can't be made driving in 'draw in view'. If I'm wrong and someone could tell me how that would be great.

I forgot to say before I'm still on V19 if that makes a difference.

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[donyoung]

Ken,


When in 'Draw In View' mode and:

- you draw a circle or a line and dimension it to an
edge of the derived model then this dimension can be made
a driven or a driving one.

- When you place a DatumTarget (by function) in free space
(but inside the model) and dimension it to an edge the dimension
is a driven one. So the DatumTarget will stay on that coordinate
(that's what it is for in this case)

- When you attach a DatumTarget to a (center)Point or an edge
of the derived model it will stick to that edge

dy

 

[KENAT]

don, I just tried the first one in your list and couldn't make the dimension driving. When I looked up help yesterday I got the impression this wasn't possible.

If it is possible is there an option somewhere, the button up on the ribbon bar is greyed out.

KENAT,

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[donyoung]

Ken,

First: the Option 'Maintain Relationships' is OFF by default
thats's why the button is grayed out. To change click on
Tools --> activate 'Maintain Relationships'. Now it will
work.

would this be a solution to your problem?
Ccreate a sketch in your 3D-model and tie it to the model. On
that sketch place tiny circles say 0.1mm at the locations where
you want to place the DatumTargets later on. Dimension them
appropriate. Rename the sketch so that the purpose of it is made
clear to someone else
Now in draft display that sketch (view's properties) and
in 'Draw In View' place the datum target (Point only) on
the center of the circles. This way the model will control
the position of the datum targets and thus you have a
single point of control.

dy

 

[KENAT]

don, that's more or less what I started to do yesterday. I didn't put the actual datum target draw in view though just on the face of the drawing but it seems to be working.

Thanks for the 'maintain relationships' reminder, that's what I was trying to find, I thought there was something like that and was searching in help for it but found someting that made me doubt myself instead.

KENAT,

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