Sketching

[MattUK]

Coud someone please help me out with sketching...basically I am sick of drawing a complex shape and when I want to make some modifiations or add other lines etc....the bloody thing always changes (drags itself) I have waisted many hours on drawings and over a peiod of changingdimensions of linesthe whole thing changes. it is extremely frustrating.


How I can draw lines shapsesso they DO NOT CHANGE what ever I change around them, somethimes the whole drawing can move on the page, and that then will be out of place in an assembly


Sorry to rant but I have been working on some parts and sketches and I am finding thatthey change shape and I cannot put them back

Thanks very much for your time


Matt.



Edited by: MattUK

 

[jeff4136]

You are talking about part or assy sketcher operations?
Use of the word "drawing" ("somethimes the whold drawing can move on the page") is confusing.

Back to model space sketcher mode: I wish there was a way to Lock Forever dimensions, but have been told by PTC tech support it's not likely to happen (couple years ago).

What I do: When going back into a sketch to modify, set the selection filter to "Dimension", window select and Lock.

If you have a few dims you want to make sure never get messed up, create relations to lock them in.

Mebbe someone has more or better suggestions?

 

[MattUK]

Thanks for the reply jeff,


basically I am drawing lots of parts and putting them together in an assembly, when I assemble the parts I notice I need to make some changes, so I open the part up and use the skether to modify...but every time it modifies something I dont want to change...I have been using hte dimension option BUT it still lets the sketch change to and unwanted shape or size ??


How CAN I lock every single line or shape I have drawn?


Thanks for help jeff


Matt.

 

[jeff4136]

> How CAN I lock every single line or shape I have drawn?

I'm not entirely sure what you mean.
Lock every entity in a sketch? Already covered.
Lock "everything"? No can do. Makes me wonder if the problem isn't changes due to normal parametric relationships that you don't expect?

> I have been using hte dimension option ...

Again, not sure. Do you mean you have been window selecting all dimensions, RMB, Lock?

> but every time it modifies something I dont want to change ...

If you have all the dimensions in the section (sketch) Locked, nothing should change except what you change and then only if can change without conflict.

Maybe we need to make sure we are on the same page...
What version of Pro/E?
Intent Manager On?
Are you making changes via Edit or Edit Definition?
Are you just starting to learn Pro/E?
Any other experience with a parametric system?

 

[MattUK]

Wildfire 2


Intent Manager on ?...dont know what that is ?


Making changes via Edit Definition


I have just started learning


No experience with parametric system


Sorry to ask jeff...how does one LOCK dimensions ?


Again I appreciate you time..sir





Matt.

 

[jeff4136]

Ok, now we're cookin...

Intent Manager (default On) is the sketcher constraint manager. It's possible to turn it off, but you don't want to.

Sketcher dimensions are Locked if you assign a value or RMB, Lock. When you modify a sketch (Edit Def), zoom out, set the entity selection filter (lower rt screen) to Dimension, window select all dimensions, RMB, Lock, set selection filter back to All.

I would recommend that you keep section sketches (or sketched datum features) simple enough that you can manage them, even if that means creating multiple sketches with dependancies. Generally, using multiple, simpler geometry constructs will serve you better than fewer, more complicated features.

Look up and go thru tutorials before you jump into trying to create any complicated geometry on your own or floundering around trying to "figure out how it works". You'll be happier for it.

 

[jeff4136]

... oops, Matt, led you astray.

Said "dims are Locked if yu assign a value". Not true unless you set sketcher_lock_modified_dims = YES. Default is NO.

 

[Dell_Boy]

A couple of suggestions.



As Jeff said, try to avoid complex sketches. If you can, break them
down into a few simpler sub-sections. If your sketches need to become
complicated, exercise them to check that ONLY the assumptions you want
made, have been made.



Don't mix very large elements and very small elements in the same sketch.



Edit the sketch definition in part mode rather than in assembly mode to
avoid Intent Manager trying to latch on to references in adjacent parts.



If necessary, sketch out of proportion. Eg sketch a line 10

 

[jeff4136]

Good suggestions, DB.

Thought I might add (re 1 degree off horizontal and constraints in general); any time you see a constraint glyph while "rubber banding" around you can RMB and it will dis-allow the constraint. You can also shift+RMB to lock in constraints before finishing the curve. It's a very cool feature.

Some time back I wrote a short essay on sketcher characteristics for a fella (Inventor user) that might be good "keep in the back of your mind" stuff for newbies. It's posted at www.mcadforums.com/forums/viewtopic.php?t=2848

 

[Dell_Boy]

Jeff,



thanks for the tip. Something new to be learnt every day.







DB

 

[Zaki]

< = defer>



Hi Matt