snapping to things outside sketcher

[2ms1]

In sketch mode, how do you snap things (ie make sure they line up with) to things in the part that were not created within the sketch you are working with?


For example, lets say you had a datum plane in your part model that ran through two datum points. Then let's say you went into sketch mode to draw (on the datumplane)an arc that connected the two datum points.


The datum points aren't actually in the sketch, of course, although you can see them. Is there any way to snap to them even though they aren't within the sketch?
Edited by: 2ms1

 

[puppet]

sketch --> reference.

select what you want to reference, You can then snap to these items.

just remember that ur now making ur sketch dependant on those references.

 

[prohammy]

2ms1,


Just a cautionary note (following on from what puppet has said), if you are using a PDM system then you may want to be careful with the above. Referencing sketches using SKETCH-->REFERENCE creates an external reference for that sketch/part. Most PDM systems do not like this (it causes significant increases in retrival time).


If you want to keep your system administrators happy, once you have finished using the ext refs that you have created to complete the sketch, go back and delete them, and either strengthen what ProE sets up as 'weak' dims or put in your own more meaningful dims


Kev

 

[2ms1]

thanks for the suggestions. Yeah I had known about that method of bringing in external thingsby adding asreference, however it had concerned me just because I'm bit of a beginner but have already gone through some hell with "spaghetti bowls" of references. Heh, for some reaons I hadn't thought of the idea of simply deleting them afterwards. Thanks guys.
Edited by: 2ms1

 

[AHA-D]

Just a cautionary note (following on from what puppet has said), if you are using a PDM system then you may want to be careful with the above. Referencing sketches using SKETCH-->REFERENCE creates an external reference for that sketch/part. Most PDM systems do not like this (it causes significant increases in retrival time).


If you want to keep your system administrators happy, once you have finished using the ext refs that you have created to complete the sketch, go back and delete them, and either strengthen what ProE sets up as 'weak' dims or put in your own more meaningful dims


Kev

What you say is true when working in assembly context. Referencing other parts while designing one part creates references among different parts.


What the OP mentioned was usings already designed geometry of the part to define new features. This only creates internal references in the part file itself an as such does not generate any overhead.


I would in no way delete these references. My philosophy is that this is what parametric modeling is all about : intelligently attaching features to others, creating interdependent parameters, in such a way that when base features of a part change other features adapt to create a new part that is functional equivalent to the original design.


As an example : take a cube and make a circular protrusion on top of one of the faces. Now you want a cutout on the opposite side that is axially aligned with the protrusion. "Safe mode" would be to dimension the cutout to base datum planes. "Intelligent mode" is to make a reference to the protrusion and use this as center. In "safe mode" you have to remember to change both protrusion and cutout parameters, in "intelligent mode" the cutout follows the protrusion, as this was design intent.


Remark : Unfortunately there's also something like "resolve hell" when your model blows up because of missing links. There's two reactions to this : seek shelter in safe mode or really intelligent AND robust modeling, looking carefully at what references what.


Alex

 

[prohammy]

AHA-D & 2ms1,


AHA is correct (teach me to not read the OP) Ref'ing geometry in a part is the corrrect way to model. What I was talking about is creating ext refs in assembly mode. Sorry for the confusion....(ext refs in assembly mode are one of my most hated things, they make my blood boil

and I think I may have got carried away here)


Kev