Lost visible lines in SE draft

[Bluejaydk]

Urgent problem!

When i make a draft of an assembly i often have the problem that visible lines of various parts is missing. (all versions from 14 to 17). I can make it show the hidden lines of the part, but not the visible.

Sometimes the drawings are next to useless, so it's pretty infuriating.

Best regards
Jesper (Bluejaydk)

 

[fwc]

Hi

Did you check Process part intersections, under General Tab in Drawing View Properties dialog box?

Regards

fwc

 

[Bluejaydk]

Hi fwc

I never noticed this function, so thank you.
It didn't help thoug. It feels like a big bug in the software. It is totally random what parts it happens to.
par-files as well as psm-files. Iso-views as well as orto-views

Best regards
Jesper

MORE CLUES ANYONE ? Anything is wellcome

Thank you

 

[Kenny_G]

Open the assembly and on the parts that are not displaying, lok at there occurence properties and make sure the option "Display in Drawing Views" is checked. If not, check it and problem solved.

Ken

 

[Bluejaydk]

Hi Pellaken

This was checked, but thank you for your answer.

It is not all of the part that i missing. Could be an axel
that is only shown by it's ends in an ISO-view. (Just an example of many)

Am i really the only one who has encountered this problem ??


Best regards to all

 

[beachcomber]

Turn on tangent edges and/or hidden detail in the view, if that doesn't work try clicking the 'Display Edges' icon.
All the hidden edges on the sheet will be displayed in the highlight colour (usually purple). If you see the ones you want, click on them and they will probably appear as hidden detail style.
Then use the 'Edge Painter' icon to change them to visible style.
SE sometimes gets confused on what is visible or hidden, or on silhouette edges, especially on iso views of revolved or circular features.

bc

 

[Bluejaydk]

Thank you beachcomber.

But unfortunately i have drafts where the amount
of incorrectly displayed lines is so huge, that
it would take days of work to fix.

I can only hope that the problem is less
significant in newer versions.

Unless someone has revolutionary news, i think i
will close this thread.

Thank you all for your contributions.

 

[Folke]

I tried a similar situation, which occured because some of the parts in assembly were placed intersecting eachother. The only way i could get SE to display the edges was to drag the parts apart or make relationships such as tangent or connect. -I'm positive that you will only find this error when making a draft based on an assembly or weldment.

 

[fwc]

Folke
I've suggested the solution to this problem on the first post of this thread.

Bluejaydk
Is it possible for you to open the files in other computers?

Regards
fwc

 

[beachcomber]

One last thought, have you tried changing the tolerance setting for the visible edge display ?
Right click on the drawing view and select Properties.
At the bottom of the General tab uncheck the 'Let Solid Edge determine VHL tolerance' and select a more accurate value.
Also check whether you are using simplified parts.

bc.

 

[fredericmenage]

Hello,

Just to let everybody know: I saw the file and it seems to have happened with V14 (update 6 I believe) at view creation.

It updates correctly in V16 and V17 (all the missing lines are added). I did not test in V14 so I don't know if any of the suggestions on this thread worked (process intersection, hide a part and update the view, ...) but it worked in V16 and V17.

VHL tolerance is not an option in V14 since it was added in V15. I advised Bluejaydk to upgrade or at least to download the latest update (update 14 for V14) if possible and try our suggestions.

Fred

 

[johnson0182]

Hello,

I have had the same issue numerous times.

Turning on process part intersections helps tremendously, but the only way to get the lines back in the drawing is to go into the display properties of the view, then turn the parts that have lines missing to not visible. Then, update the drawing view. Next, go back into the drawing view properties and turn the part back to visible. Then update the view again. I believe it is caused from SolidEdge choaking when it is creating the view. I only see the problem when creating assembly views never when creating single part views. This will save you a lot of time over creating the views again.

Jermiah

 

[donyoung]

Hi,

when I do encounter this and activate 'Process intersections'
with 'Create all face intersections' and then quit with OK
I only have to 'Update Views' to see the lines (V17)
Pressing F5 (refresh) won't do it.

dy