Offset behavior in sketcher - options to control it? 2

[Albigger]

In sketcher, when I use the offset command from the transformation toolbar, it will offset it the amount I specify but it does not create a constraint. And for instance, if I do this to a chain of lines & arcs, and I want to change the offset at a later date, I have to go back and constrain each line/arc individually.

Is there a setting I am missing somewhere to automatically create these constraints?

Pattern and rotate behave the same way, they are just "dumb" geometry after you use the feature.

I am running R19SP2.
Thanks.

 

[TAZ69]

AL,
while in sketcher under the sketch tool bar make sure your
dimensional constraint toolbar is on.

 

[Albigger]

TAZ -

Yes I have both dimensional and geometrical constraints turned on, but no luck.

 

[TAZ69]

Al,
Sorry thats the only way I can create that scenario. The only other 2 thoughts that I have are: Tools>Options>sketcher>the constraints checked (see Jpeg)
or the create datum toolbar is activated (the lightning bolt)

Sorry Hope you figure it out ;/

 

[Albigger]

Yep, I also checked those options in tools-options-etc... and they are all checked.

I'll make sure about the create datum icon when I get back to work tomorrow.

But, just to be clear, when you do an offset of say 3 curves, it normally creates a distance constraint between the original and the offset that you can later modify?

CATIA has always behaved this way for me, so if it should not be this way, I would really like to know why. The weird thing is, when i create a spline and offset the spline it will create a constraint, but not for lines, arcs, etc...

I guess I could try clearing my CATsettings too, maybe I'll try that tomorrow also.

 

[jackk]

My experience is that when offsetting a single element (a line or spline), than the distance constraint is added. But when using propagation or selecting multiple elements, everything is offset without a constraint.

If there is a way to always get the constraint, I like to hear it too.

 

[itsmyjob]

Albigger,

You can offset with contraint only 1 element at a time. If you want to offset a complete profile then you have to go in another sketch, project the profile you want to offset (it will be as one in the new sketch) then make the offset.

Eric N.
indocti discant et ament meminisse periti ​

 

[Albigger]

Thanks, itsmyjob. In that case, however, it doesn't do me a whole lot of good, because I wanted to use the single sketch to create a pocket.

It's not a big deal, just something I do often, and if there was a way to speed it up that would've been great, that's all.

 

[jackk]

Eric...

When I tried to repeat your process with R18, I run into different problems:

1. If I project each line individually, the offset propagation doesn't work.

2. I can get propagation and a single offset constraint by trapping the entire sketch.1 to project it. But I get an error as soon as I try to add more geometry into sketch.1

 

[itsmyjob]

Jack,

[ol]
[li] Like I said the offset work for 1 element, not a selection/propagation of element[/li]

[li]In order to project sketch.1 in sketch.2, first select the sketch.1 in the tree then press the project.[/li]
[/ol]

Eric N.
indocti discant et ament meminisse periti ​

 

[Azrael]

My 5 cents, why don't you use the thick option?

 

[Albigger]

Az -

I don't see the thick option in a sketch? The purpose is to create a pocket with a constant wall thickness.

(Yes, I know I could use the "slot" function, but then I am back to 2 separate sketches anyhow, where I was trying to simplify the amount of work in the first place).

Thanks for all the suggestions and information so far though. Keep it coming.

 

[jackk]

Jay; Shell won't work for you? (it doesn't require a second sketch)

 

[jackk]

itmyjob said:

1. Like I said the offset work for 1 element, not a selection/propagation of element
2. In order to project sketch.1 in sketch.2, first select the sketch.1 in the tree then press the project

Thanks, Eric, for clarifying the little trick of selecting the sketch in the tree - that makes a big difference and the constrained offset works well for me.

 

[Albigger]

I think I understand what Az & Jackk are saying now, use the pocket with the thickness option. I should've remembered that. I will try that next time.

Thanks.

 

[Azrael]

Sorry Albigger, I should have been more clear, I meant the thickness option in the pocket feature (also available in pad). I never do offsets in sketches, messy to update if you add geometry in the sketch, so I go with the thickness option in solid features or shell, sometime I use the "thickness" feature to adjust the offset if it isn't consistent.

 

[Albigger]

No problem, glad I finally got it through my head what you were saying.

I don't know why I didn't think of that earlier, I think that will be a much easier way to construct these grooves in the future.

Thanks again.

 

[solid7]

I agree with Azrael. I will even go so far as to say that it is silly to create sketches with an inner and outer domain where the thickness is constant. Why they still teach this method in courseware and books is beyond me.

I'm a big believer that it's better to have more sketches with less information, than to have less sketches with more information.

BTW - Thick is also good for making rectangles and squares from just a single line in a sketch. (or not - sketches aren't required for solid features)

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