Offset line or rectangle...

[ledo]

Why is offset disabled when we make first sketch? Why must we make one sketch first and then use another and create edge from the first sketchand only then we can offset that edge?


Whay so complicated? It gets on my nervs. And i needed a long time to figure it out.


But still i have the question why is it made like that? Why must i use relations and not simply use offset in one sketch?


















Edited by: ledo

 

[solidworm]

This is my question too. is there a logic behind this?

 

[kdem]

The tool is used with defined geometry. In one of the classes Itook it was explained that the geometry is not defineduntil you select the check in sketcher mode. So since it's not defined you can't use it. That would be my guess as to the logic of why you can't use a sketched entity, although I agree it would be nice to have an offset tool for sketched entities.

 

[ledo]

Ok so these is a fact and these is yust the way ProE does it. So i have another question:


The main problem i see at this time is these:


I have 2 sketches for 1 section. I will use complete section from sketch 2 and i will extrude it.


And now the question:


How can i put all dimensions from sketch one to control it from sketh2? On sketch 2 there are yust edges from section 1 with no dimensionsand the only dimension is offset distance.


But i want to control all the section dimensions from one sketch. Is it possible?


Is it possible to manualy add dimension to edges on section 2 that would control dimensions on section 1?





Or its not possible and i must use 2 sketches to control dimensions of a section that have offset in it.





Section1: Dimension is diameter


Section 2: Dimension is offset distance


Is it possible to control diameter and offset distance from the same sketch?





s



Edited by: ledo

 

[davisdony]

Hi Ledo



I think u can creat all the sketch in sketch curve option.

Then while creating extrution or cut use UseEdge only



by this u will have dimentions only in one featur that is the first one

Sketched curve



hope this will solve this issue



Edited by: davisdony

 

[sip]

And if you don't want to use the outline of the first sketched line for your protrusion, but still use it to dimension to, then convert it to construction line.


Sip
Edited by: sip

 

[ledo]

Ok ill try thanks.

 

[jeff4136]

> How can i put all dimensions from sketch one to control it from sketh2?
> On sketch 2 there are yust edges from section 1 with no dimensions and
> the only dimension is offset distance.


Attempting to control Sketch_1 from Sketch_2 would not be the way I'd do it.
I think it's possible but would require two regens to update properly. Might
also end up with a circ ref and never regen properly.


Instead I'd put a Sketcher Point in Sketch_1 and dimension it the desired
offset distance and create a relation in Sketch_2 ...


sd(offset) = D(offset control dim in Sketch_1)


What is the root of the desire, though? There are, maybe, half a dozen ways
to control both sketches from some common 'place'. One or another might lend
itself to some specific application better than the rest.

 

[ledo]

Yes i thougt abaut using relations.


The point was to have all dimensions controled from one sketch. Nothing else.

 

[tommypurple2]

What if you made a curved feature before any of your features that had both sets of sketches and then in your sections you would just use the edges of which ever curves you want?


You would get an extra feature this way, but they would be controlled in one feature too.

 

[csusie]

why dont you sketch 2 circles and create a dimension that is the distance between them? Have you tried that?

 

[csusie]

No points, relations, or multiple sketches required.

 

[ledo]

Yes your method works fine. The problem is i am a begginer and firstly didn't know why offset doesn't work in first sketch.


Then i didn't know how to put diameter and offset on the same sketch so i could controll all the dimensions from one sketch.


Yestrday i learned how to make my own dimensions for the first time. (select 2 lines orpointsfor exampleand press middle button on mouse).


And today you give perfect solution. Maybee tomorow i would figure it out myself. Maybe not.


It's so simple nowthe solution is here.But the path to these knowladge was long.


Thanx for all replays and final solution.






Edited by: ledo

 

[ledo]

Update.


On circles your methode works perfect.


But to "simulate" offset feature with 2 rectangles (or triangles or n-size shapes) things get wery complicated.So for using offset we still have to make another sketch and use edges.






Edited by: ledo

 

[jeff4136]

> The problem is i am a begginer


Try creating the feature as a 'thin solid' rather than creating the second (offset) sketch?

 

[csusie]

Update.


On circles your methode works perfect.


But to "simulate" offset feature with 2 rectangles (or triangles or n-size shapes) things get wery complicated.So for using offset we still have to make another sketch and use edges.

Use construction geometry and the equal constraint for something like a rectangle. Or the "thin" solid or cut feature as suggested above is good.

 

[ledo]

Yes but if we create a solid with extrude (these how i interpreted your suggestion) we still can't controleverything from one sketch.


I camed to terms that these is yust the way proe does it and appart from circles from uper example the solution is using 2 sketches. Or the method you mentioded.


But offset isn't a option for one sketch.So if we want to use offset we need to make 2 sketches. Thats the point.


Many ways t the end but with offset we would need at least 2 sketches... These is new to me and i neded some time to understand it how its done with offset.





Bottom line: Offset in proe needs 2 sketches. (two sections).












Edited by: ledo

 

[csusie]

Offset inside of sketcher needs pre-existing geometry and not the geometry you are currently creating in the sketch. By suggesting that you are correct.


There are however other ways to get around that if need be. Otherwise there really isnt that much of a problem in creating 2 sketches depending on what you are doing.


If you are doing an extrusion or similar it is just as easy to sketch 1 of them and then use the thin option and there you would input the offset value.


If you have alterior motives for the sketch and are not using it for a sketched based feature then you may have to resort to the 2 sketches.


What do you plan on doing with this type of sketch, you have not metioned this.

 

[kdem]

Bottom line: Offset in proe needs 2 sketches. (two sections).

I would think of itas ProE needs model geometry for the offset edge to work.The geometry in sketcheris sketch geometry. The other thing to realise is that depending onthe type of geometry you are using the sketch for having all the geometry on one sketch may not be what you want. For the example of the two circles it may be okay for a washer or gasket but I wouldn't use for something like a step shaft. For that you would end up with two more sketches.

 

[ledo]

Much things makes sense i know. But if i am honest iwould like to hear official explanation of PTC personelwhy sketcher geometry does't support offset.


I think there must be a good reason to it. Mybe in the future when i will be more skilled i will found out.