trimming offset entities in a sketch 1

[antran7]

There's got to be a way... Here's what I'm trying to do:

I've got a sketch, and it consists of 4 different offset entities (i'm offseting the 4 boundary edges of a surfaces, and they're different offsets so I can make them different).

If I leave it at that, it's fine: I can modify the offset dimensions, and the entities moves as they should.

BUT: if i trim those offset entities so they form nice corners, I can't modify the offset dimensions. On top of that, the sketch is marked "undefined" (but if i didn't trim the offset entities back, the sketch would have been fully defined and modifiable).

What gives? There's got to be a way. I've even tried to leave it untrimmed, and make a 2nd sketch that coverted the offset entities and tried to trim that. But the 2nd sketch shows up as undefined, and doesn't follow the change of offset dimensions from the original sketch.

Thanks in advance!
An

 

[ctopher]

I'm not clear what your sketch looks like. Can you show a pic?

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP3.1 / PDMWorks 05
ctopher's home site (updated 06-21-05)
FAQ559-1100
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[antran7]

http://66.219.35.155/solidworks-trim-offset.jpg

this shows an iso-view of the sketch. I'm offsetting the sides and bottom, and creating an arc for the top (I had simplified my problem in the previous post).

The sketch plane is hidden, but is somewhat parallel with the top surface (the top surface is an extruded arc).

You can see on the bottom corners of my sketch (highlighted green) there are extraneous offsets that I want to trim off. The same is true for the top.

But when I do that, I can't modify the offset dimensions (10, 20, and 15mm in the sketch).

Thanks for your help.
An

 

[ctopher]

Maybe try delete the dim's, trim the lines, then dimension again. Looks like you are dim to the end points of the lines?

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP3.1 / PDMWorks 05
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[antran7]

Those dimensions were created when I made the "offset entities" sketch feature.

If I try to delete those dimensions, it warns me that "deleting the offset dimension will remove the offset relations fromt he sketch geometry. do you want to continue?"

if i do continue, it converts the offset entities to splines.

weird, huh? any clue?

 

[CorBlimeyLimey]

Try using the Split Curve tool at the intersections of the splines, then deleting the uneeded portion.


Helpful SW websites every user should be aware of faq559-520
How to get answers to your SW questions faq559-1091

 

[antran7]

Thanks for the help. I tried that, but it acts the same as if I trimmed it. I can't modify the offset dimension (well, actually, I can, but it doesn't budge the offset entity).

Now I'm trying to circumvent this problem by just dealing with the full-sized offset entities, and just make overly extended surfaces, which, hopefully, I can trim.

I'm just having to make ten times more features than I should need to.

Thanks again.
An

 

[ctopher]

Is the dim's in context of an assembly?
If so, edit part within the assy.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP3.1 / PDMWorks 05
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[antran7]

nope. it just within that part.

It seems like once you alter the offset entity, it turns it into a spline (and it may not warn you that it's doing that). So when you modify the "offset dimension", it's just moving one of the spline ends, and not really increasing the offset.

It's weird, and a pretty big oversight by the SW programmers. Maybe 2006 fixed it. (BTW, i'm using SW 2005)

An

 

[TheTick]

For what it's worth, I've noticed offset entities in sketches doesn't work as well as it used to. I've had problems similar to what you describe, especially with offset dimensions not working once offset curves are trimmed. It used to work fine that way!

If your entities are arcs and line segments, try taking the low road and use parallel and concentric constraints wit dimensions.

I could be the world's greatest underachiever, if I could just learn to apply myself.

http://www.EsoxRepublic.com

-SolidWorks API VB programming help

 

[ctopher]

try edit sketch on '(-)lcd outer', then trim lines and rebuild. Is it what you are looking for?

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP3.1 / PDMWorks 05
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[antran7]

Once I trim those offset entities, I can't modify the offset dimension. So it's a one-way trimming. If I later need to change the offset dimension, I have to rebuild that sketch, and referenece all of it's children to the rebuilt sketch.

Another weird thing is that it only become under-defefined when I trim the corners.

And another weird thing is if I trim one corner, and them modify the offset dimension, it locks that trimmed corner down and pivots the rest of the 'offest' entity around that locked corner.

Thanks tho',
An

 

[antran7]

It's just funky like that for complex offset entities. If you're offseting an arc or a line, it works just fine, even after trimming it back to other stuff.

But once you have to offst a surface edge, or a spline.... beware! It'll act funky on ya, and may by modifiable, but it's not really an offset anymore.

Thanks again for all the help.

 

[ctopher]

I trimmed the lines. I'll send the part back to you. Let me know if anything works different. thanks

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP3.1 / PDMWorks 05
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[antran7]

the lines are trimmed back, but now the sketch is marked with the 'underdefined' mark.

when i try to modify a dimension, for example the right offset on lcd-outer from 10 to 20, the dimension lines move, but the actual offset entity doesn't move.

there's no warning of failure or over/under contraint, but the sketch isn't modified, nor are the children that reference that sketch.

here's what i see:

http://66.219.35.155/solidworks-trim-offset2.jpg

does it change the sketch on your machine?

 

[CorBlimeyLimey]

After making the offset entities, close the sketch. Then start a new sketch & use Convert entities to create new geometry. Maybe you will be able to trim those.


Helpful SW websites every user should be aware of faq559-520
How to get answers to your SW questions faq559-1091

 

[ctopher]

It looks like it is moving for me.
I don't see any errors.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP3.1 / PDMWorks 05
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[antran7]

corblimeylimey,

I tried that also, but it didn't work for me. The new sketch wouldn't follow the original sketch if there were trim function. So if i modified the original untrimmed sketch, it would modify properly, but the 2nd sketch that converted and trimmed the original would re-convert the modified original. It would be stuck at whatever offset it was trimmed at.


ctopher,

I guess I've got a bugey version of SW, because when I modify those dimensions, it acts like there's not error, but the sketch hasn't really changed.

I was able to get a work-around tho'.

Thanks again,
An

 

[antran7]

ctopher,

what version of SW are you using? I'm using
SolidWorks 2005
SP0.0

 

[antran7]

I upgraded to SW2005 SP5.0, and it seems to be working now. I can modify the offset dimension, and the trimmed offset entity changes as it should.

So basically: somewhere between SP0 and SP5, they improved the offset entity sketch feature to be able to deal with complex curves.

Thanks to all that helped.
An