convert entities to section

[enriazzo99]

Good morning to all,
Today I have a problem, indeed a curiosity about the achievement of a function:
I have to make a traverse in a hopper moved by the central axis of x mm. so as you can see in the enclosed screen my need would be to be able to make a convert entity of the line that is highlighted in blue, but it is not possible being in a section. Can anyone help me?
Thank you in advance.

 

[MassiVonWeizen]

simply put the lines selection in hidden mode temporarily in system options

 

[enriazzo99]

hello in the meantime thank you for the answer, I checked and to me it seems already the selection of the lines in hidden modalities if not erro.
but when they select convert entities, they no longer let me select the lines.

 

[MassiVonWeizen]

Did you try to put the tick on your voice too?

 

[enriazzo99]

I tried to show up but nothing changed unfortunately

 

[MassiVonWeizen]

but is that a real edge or is the result of the section?
to avoid it, did you select a border or surface?

 

[enriazzo99]

I apologize maybe I didn't explain well in the first post.
that edge highlighted in blue is the result of the section I did.
to highlight it I selected the edge and not the surface.
when I enter into "converted entities" it no longer leaves me to select and not even the surface.

 

[re_solidworks]

If you do a sketch on a plane/face parallel to the section, you can convert into entity the edge that is generated in projection. in cases of complex sections, sometimes, the command does not work well and to solve you can divide the face using the line of division of silhouettes.

Creazione di linee di divisione di silhouette - 2021 - Guida di SOLIDWORKS

help.solidworks.com

Let us know if you solve it!

 

[enriazzo99]

hi, I had already tried to do a sketch on a plan that coincided exactly with the section but I can't convert to entities.
The silhouette forgives me but I can't understand how to use it. In my case, would you tell me what to put in the two boxes? Thank you.

 

[re_solidworks]

hi, I had already tried to do a sketch on a plan that coincided exactly with the section but I can't convert to entities.
The silhouette forgives me but I can't understand how to use it. In my case, would you tell me what to put in the two boxes? Thank you.

in the first box the sketch plane, in the second the surfaces you have to "divide" to get the edge you want to convert to entity.

 

[enriazzo99]

I give the parameters like you explained to me, but the line creates it along the middle floor. I need a division along that plane moved by x mm from the station. Where am I wrong?

 

[fgmec]

Have you tried to make an extruded cut where you want the section and use the edges that result to build the sketch? (then cut the gates)

 

[re_solidworks]

I give the parameters like you explained to me, but the line creates it along the middle floor. I need a division along that plane moved by x mm from the station. Where am I wrong?

the silhouette line is created on the surface. Then create a sketch on the plane where you want the convert entity and try to convert that edge that you couldn't.

 

[re_solidworks]

Have you tried to make an extruded cut where you want the section and use the edges that result to build the sketch? (then cut the gates)

when you delete the cut the contour loses the references.

 

[fgmec]

Sure. meanwhile he can see if he gets what is necessary. then maybe it will attach the sketch to some other independent element.

 

[enriazzo99]

with the silhouette unfortunately I couldn't do it.
with the method recommended by fgmec you can manage but as it said re_solidworks erasing the cut you touch me leave the sketch without constraints. Thank you very much

 

[re_solidworks]

You could also try with "intersection curve". open the sketch on the correct plane, take the intersection curve command, touch the surfaces that you will intersect and you should find the curve made.

 

[enriazzo99]

You could also try with "intersection curve". open the sketch on the correct plane, take the intersection curve command, touch the surfaces that you will intersect and you should find the curve made.

thank you so much I managed correctly using intersection curve.