Break on isometric view

2D plans Layout
1

Hello

In order to get me to encrypt duct networks, I created drawings in a hurry, that is to say that instead of making several views of my networks, well detailed, I put them in isometric view and I quote directly on them, so that my supplier has an estimate of the lengths he has to calculate and so that he can see which head to my network.
My problem is that when I want to insert a break, well the elements don't follow, they stay at the same "altimetry". Is there a solution to solve this problem??

CF Image

Thank you, Cdt,

Joss


cassure_vue_iso.png
2

Hello

 

I have the same problem with some of my iso views.

 

What I do is I make my break, and then I put in as little space as possible.

 

But hey, it's still DIY... ^^

3

I do have one... You insert another break perpendicular to the first one that you adjust to have a coherent visual.

Otherwise, I rather do classic pieces (Face, Top, Left) and I link the breaks (so as not to have a gap between the views).

2 Likes
4

Otherwise, you have to trim your eyesight as attached.

 

For me, it's the best solution =)


rogner.png
5

it looks like this =)

 

Then you just have to set the space you want on your sketch


rogner_2.png
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@Bart, trimming doesn't visually decrease the length of the part like a break? No? :)

7

@Benoit, reducing the space between the breaks to a minimum does not change their altimetry, which is a shame, it does not change much :(.
And I don't find it very interesting (at my level) to make several views, it would waste a lot of time when it's really for an approximation of lengths that I need to rate my networks...

@Bart, concerning the cropping, if I reduce the space in my sketch, it will not bring the two parts of my part closer together, whereas I made a break to reduce my part and avoid putting myself at 1/75th instead of 1/50th.

8

why not make your breaks on the main views

See this link

http://help.solidworks.com/2011/french/SolidWorks/sldworks/LegacyHelp/Sldworks/drawings/Section_View.htm

 

@+

 

1 Like
9

I have trouble expressing myself. :/

On your iso view with vertical break, you add a horizontal break. Visually you will be able to catch up with the level.

Look at my image of a tube

1 Full view

2 Vertical break

3 Addition Horizontal break on top of vertical break

It seems to be what you want.


screenshot465.jpg
1 Like
10

Indeed, right now, I'm drying... ^^

11

@gt22, the link leads to section views, I don't really see the connection with my problem in what I read :-/ (maybe I misread??).

@Benoit, then, several problems in your proposal: first of all, whatever I do, if I make two breaks, if I change the interval of one of the breaks, automatically, the other one takes the same interval, which means that I am never aligned. And then, I can't make horizontal breaks because my network is cut on all sides (see image)

 


cassure_horizontale.png
1 Like
12

Oh yes, with a broader view I understand your concern better!

There, I don't see a quick solution :/

13

Sorry

Here is the link to the breakout line

http://help.solidworks.com/2011/french/SolidWorks/sldworks/LegacyHelp/Sldworks/drawings/HIDD_DVE_BREAK_VIEW.htm?id=af41de78b3a4496695ee7d1a485d5431#Pg0

 

2 Likes
14

Set the full iso view

Add a break

Make a CTRL+P

Take out your pair of scissors and a roll of tape, gather them together

And scan :p

 

Solidworks Practice ^^

2 Likes
15

Not bad the scissors stroke, I hesitate to put you in a better answer;D

@gt22, haa yes, it would have been not bad but I have another problem, the view I put on my drawing is the view that allows me to see the maximum number of elements of my network and therefore, it's an iso view but of the "View in progress" and I therefore don't have a parent view:(

16

After a long search, no solution possible, the help of Solidworks and the other forums do not give :(

17

Hack in Bart's idea: make 2 cropped views and align them (more or less)

1 Like
18

Hello, I'm coming back to this post because I had the same problem.

I don't know if it can help anyone. But here is the solution I apply to make breaks on my isometric or non-2D views on my drawings.

1)  I don't make the break with the "break" tool on the drawing (otherwise the 2 pieces are not aligned),  but I create the break on the part in 3d (or on the assembly) with "View of the model break" (Insert menu)

I choose the breakout space by moving the 2 breakout planes

2) I validate, the part is split and this creates a new Configuration of the part in the ConfigurationManager tree

 

3) I insert this view into the drawing, Insert view of the current model (or other) And I right-click on the view, property and I check "Show in exploded or broken state of the model".

And here's what it looks like:

If it can help someone, it makes my drawings easier because I work with fairly long metal profiles and a split view in isometric (or slightly biased) is clearer for the clients.

 

PS I use SW2016 sp3, I don't know if the previous versions have this function

Cdt

Anthony