"implicit" sketch relations

[dgowans]

Can anyone enlighten me as to how I can make a sketched line totally unencumbered by sketch relations - either implicit or explicit? I've got a sketch that I used in my first revolved feature that now needs to be modified to have draft incorporated. I've deleted all relations from the line - and its endpoints - in question (with the exception of the associated offset entities/relations) such that I feel that I should be able to drag its endpoints so it's no longer vertical. No dice.

I've tried adding a construction line at an angle to this line, adding an angular dimension (my desired draft angle), and then adding a vertical relation to my new construction line, thereby hoping to force the initial line to have my desired draft. No luck there either.

Now I know that I can add draft features or delete the offset sketch entities/relations and get what I want. In this particular part, fixing any rebuild errors wouldn't make this a show stopper, but if I had a complex part where I would lose a lot of time fixing rebuild errors, how might I go about this? I've run into this in the past and never come up with a bullet-proof method of making a sketch entity totally unconstrained.

Thanks in advance for any advice.....

 

[ctopher]

Have you tried selecting all the lines in the sketch, copy, create a new sketch, paste, delete old sketch? If I understand correctly.

Chris
Systems Analyst, I.S.
SolidWorks/PDMWorks 05
AutoCAD 06
ctopher's home site (updated 06-21-05)
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[dgowans]

Not sure I understand how this will help.

What I'm trying to avoid is losing relationships between my first feature and any downstream features. I know there are any number of ways to get my part to look the way I want, your method being one of them, but I'm trying to do this with a minimum amount of rebuild errors. Your way, I believe, will lose relationships to everything built off the first feature.

 

[Theophilus]

Sounds most like you still have some parallel or vertical/horizontal relationships remaining. I run into this all the time, and try to do what you do for the same reasons. You can succeed at this. Select the line you want to change and you should see the relations display on the left--delete whatever is constraining your line. Then do the same for each point of your line, just to make sure they aren't the problem.

Jeff Mowry

http://www.industrialdesignhaus.com

Reason trumps all. And awe trumps reason.

 

[CorBlimeyLimey]

"(with the exception of the associated offset entities/relations)"

What happens if you delete those?


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[dgowans]

Theophilus,

Yep - I've done that. What I believe is happening is that the offset relation on my line in question is screwing me. I can go in and remove every relation on the line and its endpoints, including trimming the line away from its adjacent sketch entities so there are no implied relationships on the endpoints. Blue line, blue endpoints. What I have at this point is an unconstrained line that has an associative offset entity. What I would like to do is then modify my original entity to have draft so that my associative offset also has draft.

CBL,

I'm trying to avoid deleting the offset relations, basically because I don't think it should have to be done this way. I suspect that I can delete the relations on the offsets, make my changes to the initial entity and redimension the offset entities, but why should I have to do that? On a complex sketch that would be a real time waster. I simply want to modify the angle of my initial line and have the offsets update accordingly. It appears that the tail is wagging the dog in this instance.

Consider this my addition to the thread on things that drive me nuts...............

 

[CorBlimeyLimey]

I just made a simple sketch, (rectangle with an offset rectangle), then deleted the vertical constraint on one line (not endpoints) and was able to move the line off of vertical. The offset line stayed offset & parallel to the moved line, so it does not appear to be the offset which is causing the problem.

What SW/SP versions are you using?

Can you post a sketch or the file?


Helpful SW websites FAQ559-520
How to get answers to your SW questions FAQ559-1091

 

[dgowans]

SW2006 SP4.0 - I'll see if I can replicate what you did, otherwise I can post something....

 

[dezignstuff]

If the offset entity has relations to something outside the sketch, or if it is Fixed, it will prohibit the original entity from moving. If the only relation in your sketch is an offset between two sketch entities in the same sketch, then there is no reason why either of the entities shouldn't be able to move.

If you have an unsolvable or zero length entity, or some sort of converted / offset spline entity, the problems you describe are completely possible.

Try to overdefine the sketch to see what is going on. If you force something that should work, and it overdefines, just see what it is in conflict with.

Of course you can't exclude the possibility that you've run into a bug. This happens to me all the time. 2D sketch relations, as basic and as commonly used as they are, are still one of the buggiest areas of the software.

Possibly if you posted your model, someone could help you out.

 

[dgowans]

http://multiterra.mooload.com/file.php?file=files/180406/1145382504/sketch_relation-modify.SLDPRT

is a SW2006 part containing only the sketch in question.

 

[rfus]

It comes down to fundamental sketching practice. Convert entities and offset entities, like flaming shots of 151, seem like a good idea at the time, but pretty soon everything goes up in flames. When I see new users they will use these tools religiously. If you wipe out a sketch and recreate it you've screwd youself down the line. Once you've been burned enough, and are tired of seeing red or brown, you find ways of creating relations that will carry all the way through.

Offset controls the endpoints. You cant change them.

Can you delete all offset relations and create individual relations and dims on the profile. This does becomes tough when offesetting splines, but... for everthing else use offset to create the profile, but then delete this offset dim, everything goes back to blue, and go back and use relations and dims on each sketch segment to keep the parent/childs.

RFUS

 

[dgowans]

Offset controls the endpoints. You cant change them.

Really?!?!?!? Not questioning you, but this seems like a fundamental error in how the offset command is written. Then again, it does seem that SWX puts constraints on endpoints when constraints on lines would be better (think symmetry constraints when mirroring sketch entities).

When I first learned 3D, way back on I-DEAS v. whateveritwas back in 1992, I was taught to dimension from line-to-line whenever possible rather than line-to-point or point-to-point, simply because dimensions to points, in absence of other relations/dimensions, had an infinite number of solutions.

Anyway, I think we've all wasted enough time on this....

Bad Offset command - go to your room!

 

[rfus]

I meant only in a sketch where everthing is offset, thats kind of a duh statement. Yes you can offset, delete one of the offset relations, and move the endpoints

 

[dezignstuff]

if you offset a single entity, you can still drag the endpoints, even though they're black. If you offset a chain, only the shared endpoints where an offset entity is on either side of the endpoint will be immobile.

 

[dezignstuff]

Thanks for posting your model. Your problem is because you have dimensioned to the line itself, so because the dimension is a linear dim between two entities, and one of the entities is Vertical, the other is forced vertical as well.

To fix it, first delete the vertical relation (vertical 4)on the line, select the dimension, and drag the handle at the witness line up to the endpoint. The line should turn blue and now you can angle it.

By the way, have you ever given any thought to using thin features rather than offset sketches? That would be a better solution to the problem, in my opinion.

 

[dezignstuff]

The dimension I'm talking about is the .563 dimension. It changes from dia to radial when you drag it, so you will have to rmb on it, Properties, Diameter dimension.

 

[dgowans]

Interesting - that works on the .563 dim, but I can't get it to work on the .850 dim. I can delete the relation, drag the dim (now .425), but I can't drag the other endpoint to get my line to angle.

Thin feature would work, of course, but again, that wasn't my question. I was trying to modify what had already been done. Seems to me like Solidworks is a mature enough product to be robust enough to allow me to tackle this. I'm in the conceptual stage of this part design, so I was playing around with some stuff to see where it fell. This sketch had initially been a solid revolve with some cuts hogging out inner material - I seem to remember that you can't change a solid revolve to a thin feature - at least not easily.

This is my entire point - I should be able to modify my sketch to get what I want without having to jump through hoops.

Not to get this thread going off in another tangent (but I will pose the question anyway, if there's interest I'll start a new thread, which may ultimately lead to an enhancement request....), but would anyone like to be able to change a feature from one type to another? For example, change an extruded boss to an extruded cut? I-DEAS has (at least before the merge w/UG) this capability, and it's pretty slick for conceptual stuff. Once you've completed a sketch, you go into a form for Extrude, where you can join, cut, add (the equivalent of deselecting the merge bodies option in SWX), intersect, and a couple other Boolean type operations. If your part design changes, or you simply hit the wrong option, you can edit the feature and change it to what you now want. ER, anyone? Not that this would be a small programming change, but I for one would like this functionality.

 

[rfus]

I've used Cimatron, and this type of open architecture modeling, where solids and surfaces are treated the same, is really nice to work wtih, and you can grab a feature and slide it back and forth as a cut or boss, but I can essentially do the same thing with solidworks if I design with surfaces or create two solid features with the same sketch and toggle thier supression. I believe after using SW enough you start to say the opposite. Why can't CAD package X do this, because solidworks can.

 

[ongybill]

Back to the original question. The easiest way to totally remove all sketch relations is to click VIEW, SKETCH RELATIONS.

This will show every stinkin relation in the sketch in a little blue box. You can then click on the individual boxes and delete them.

Much better then blindly hunting to find relations you can't see and aren't sure are there.

I'd really like to see a simple command introduced <Delete all external sketch relations>. But individual deletions work, just slow.

 

[ongybill]

Oh, forgot to mention, if your sketch is flagged because of a bad or missing relationship when you show the sketch relations the BAD FLAGS will be red. If you delete just the red ones the flag goes away.