sharing a same sketch between several parts

[Per5]

Good morning to all,

I would have the need to share a sketch of a part to create a second, using as a starting point the sketch of this first part.
the simple copy and paste into a new file doesn't suit me as I would lose any kind of relationship between these two sketches.
I would be very useful for this report to remain in such a way that by changing the first part of it, I would also be altered by the second.
Do I have to build the part on the axieme or are there better and simpler systems?

 

[MassiVonWeizen]

try if exporting the or the bodies you have the possibility to export even the sketches.
or in one. new part insert the existing one including sketches. eliminate the bodies of the part inserted and work on the sketches

 

[Per5]

Okay, thanks now I try. but to export what I have to do, what is the command?

posted by my redmi note 2 using tapatalk

 

[sweep]

I do this:

1) I create a part and design the sketch that I will need as a basis for the creation of the other parts and save.
2) I create a part and insert the previously created part, menu insert---part.

I repeat this operation (2) for all the parts I have to create and which must refer to the sketch of the first part created (1).
the advantage is that the changes made to the sketch created at point 1 find them, almost automatically, even in the parts created at point 2.
as you see, I didn't create any together.

 

[MassiVonWeizen]

Excuse me, but what's the point of making these imports? What does it take between having a set and a part with sketch if always a file you have to carry behind? for me it seems more convenient to create and save from together than to create, close and insert a part in one part. I'm curious.

 

[Per5]

We are doing some tests on what will be more comfortable, at the end of all, we will probably realize that it is better to build the part directly from the set. Together we perceive a certain difficulty in taking the sketches that we are interested in related to details to look for in the component tree. working only with what interests us is easier. Consider that we only did a basic course, so all the rest we are experiencing.

posted by my redmi note 2 using tapatalk

 

[sweep]

Massivonweizen,
I agree with you that the environment together is the most correct one to assemble the parts, but in the request of per5 I have grasped a more specific need. I understood that its need arises from the fact that some parts that compose and interact together have the need to coincide with common sketch entities.

 

[MassiVonWeizen]

I also previously responded to the specific request, but then I grew the curiosity of what motivation can be behind, motivation that could be born a tomorrow to me too.
However, I did not speak of the correctness of the procedure, which is valid in the courses, but when working one must get dirty the soul, but of practicality.

 

[Per5]

Anyway, I was useful. so thank you for the advice.

posted by my redmi note 2 using tapatalk

 

[pritio72]

...I wanted to re-enter this discussion; Assuming that coming from pro-and the sharing of the surfaces and the management of the skeleton was more simple to me. I found myself creating a plastic handle+ rubber that for plastic molding needs is divided into 2 semi_sponges. now I have created a part of superfice + various references that represents the grip style; then I create a new part and insert inside the style part and start working. in this way if you have to change the grip style the part regenerates without problems. then if this is the most correct procedure I don't know... it worked to me and the various modifications of the all-in-one style are reused to manage them well.
View attachment 46241style created as part
View attachment 46244new part with interior style
View attachment 46245final part - obviously assembly plastic+ rubber.

we say that with pro-and once you created the style with "public surfaces" you came to do this.
If you have other methods... it would be nice to share them.

 

[pritio72]

style created as part
new part with interior style
final part - obviously assembly plastic+ rubber.

 

[sweep]

Massivonweizen,
You're right, it's not a matter of fairness, I used an unrestricted term. my first answer was focused (at least that was my intention) on the request of very clear per5 in the title he assigned to this discussion.

 

[CIARLY]

Good morning to all,

I would have the need to share a sketch of a part to create a second, using as a starting point the sketch of this first part.
the simple copy and paste into a new file doesn't suit me as I would lose any kind of relationship between these two sketches.
I would be very useful for this report to remain in such a way that by changing the first part of it, I would also be altered by the second.
Do I have to build the part on the axieme or are there better and simpler systems?

another system to share a sketch is to save it as a library function.

it should be done the sketch in an empty part, and it is saved as a library function, then this can be recalled in several parts by popping up "maintain connected to the origin"
at that point the changes to the function reperquote on the parts.

 

[MassiVonWeizen]

thanks ciarly.

 

[Simon771]

save the sketch as a block and use it every time you need it?

 

[MassiVonWeizen]

save the sketch as a block and use it every time you need it?

No.
Is there nothing to do with each other? http://help.solidworks.com/2013/italian/solidworks/sldworks/c_library_features.htm

 

[CIARLY]

save the sketch as a block and use it every time you need it?

the block when you call it back does not remain connected to the origin which means that it does not update, so you lose the chance to make changes.

 

[Simon771]

Exactly. Ideuzza shit my :biggrin:

 

[malf]

derivative sketches in axieme environment:
part a and part b together
- creates the "guide" sketch in part a
- poniti in modification of part b, but always together
- select a part plan b and the "guide" sketch in part a with ctrl
- insert-> derivative disk

is created a new sketch completely locked internally. . all content is the exact copy of the first sketch and remains connected in the changes. the only modification you can make in a connected sketch is to fix position and angle of the whole design as it was a unique rigid block.
of course the connection is managed by the reference assembly, if you change the part a, part b does not notice so long that the assembly in which the connection is created is not opened.


If the sketch is simple, however, I often happen to redesign it in part b and impose equal relationships between its elements and the homologues of the sketch of part a.