Using Break Out command

[MikeKovacik4928]

Hi everyone

Haven't used this command very much before. I am needing to use it extensively now.

Having great difficulty in figuring it out.

I am wanting to breakout a portion of a view from one particular position (or  plane) to another .

I do my "breakout" sketch on the master (front) view, for the piece I want to remove.

on the projected side view I then invoke the "breakout" command, and on the depth choose a point and enter a distance.

The break out then happens  and I then project an isometric view which 

is linked and shows this on a "3d" view, which I am using for a parts catalogue.

This however doesn't allow me to remove the portion I want. It starts right at the front of everything, and goes back

some arbitrary distance, which doesn't even seem to relate to the distance I entered.

I need some help here.

Can anybody explain in detail or point me to some nice simple explanatory videos or tutorials showing actual examples

Mike Kovacik

South Africa

[-niels-]

@MikeKovacik4928 I'm actually doing the same thing at the moment and i had the same issue.

Here's the, rather involved, sequence i've found to create "positional breakouts" in my isometric views:

1. Create a view where you can position your breakout as desired
2. Create the sketch and breakout to the desired depth
3. create an isometric view of this base view, disregarding it's orientation.
4. edit the isometric view, you won't have a viewcube which we need to fix
5. go to the "display options" tab and deselect "orientation from base" + all the "cut inheritance" options
6. now you should be able to reorient the isometric view as desired.
7. make sure the re-activate the "cut inheritance" options to get the break-out again.

[MikeKovacik4928]

Thanks Niels

That's about what I am doing.

Thanks for the info about the "orientation from base " settings. I never knew about those.

However it still doesn't give me the option to do "custom view orientation" where the break out is not lost.

When the "orientation from base" is switched on my break out is there.

When I switch it off my breakout disappears and I can do the custom view orientation.

After finishing the custom view orientation, I now need to get my break out back again.

So when I switch the "orientation from base" back on again, the break out comes back again,

however my view switches back to what is was before I did the custom view orientation and I am 

back at square one again.

Also I still haven't figured out how to do a break out from one point or plane to another,

not through the whole part like you have done (your part is only a thin plate)

mine is a complex assembly where I don't want to go through everything.

I don't know whether this is possible.

Mike

[-niels-]

@MikeKovacik4928

I think what you're trying to do should be possible.

First off, with a custom orientation, don't enable "orientation from base" again.

Only enable the "cut inheritance".

(this works, i tested it to make sure)

As for the issue of cutting through everything, i think this can be done by either defining your break from a different base view. (if you use a side view, try from the top)

Or, just let it cut through everything and then alter the "section participation" for the parts you don't want cut.

(enable part selection, right-click on the part you want to exclude and look for "section participation")

You have to disable the section participation in the base view, not in the isometric view (or custom orientation)

(this is a quick example, i'm using a see through color for most of the parts here but i hope the intention is clear)

[-niels-]

@MikeKovacik4928 here's a bit more complex example of something i'm currently working on:

The bottom view off-sheet to the left has a custom view orientation in order to cut away everything to the right of what is shown.

From that i created the off-sheet top view in order to cut away into the belt and sides.

Then from that view i created the isometric view where you can see it inherited all the break-outs.

Hope that helps you in your endeavors.

[CGBenner]

@MikeKovacik4928  Did the information provided by @-niels-  answer your question? If so, would you please use Accept Solution so that others may find this in the future? Thank you very much!