Hidden Line View on Selected Objects

[MikeKovacik4928]

Hi Inventor Users
.
1 Use the show/hide hidden edges
 function to manually
select each hidden line that
I don't want to
appear (shown in red).
In this case it is really only the
hidden edges on the one component
that I don't want to see
.
This is quite a time consuming process,
but in my opinion well worth the time and
effort, to make the drawing much more
readable

.
My  question is
.
TO OTHER INVENTOR USERS
.
1. Do a lot of other inventor users do  this, or am I in the minority
.
IF I AM NOT IN THE MINORITY I WILL PUT FORWARD AS AN IDEA
when changing views to hidden line, you can select which parts you
want to show as hidden line, and the others you don't select get left
as hidden line removed.
.
Michael Kovacik
2d & 3d Autocad and Inventor designer/draughtsman
.
Draughting/Designing (Manufacturing) (31 yrs)
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--Cad (28 yrs)
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---AutoCAD 2d & 3d (16 yrs)
---Inventor (4 yrs)
---Autocad and Inventor Simultaneously (4 years)
---(and recently Autocad/Inventor Customisation)
.
Higher Diploma Mech Eng
Ex Member SAIMechE
Technician Member ECSA
Collaborator (Rank 9) on Autocad & Inventor Forum
Certified Autocad 2013 & Inventor 2013 Professional
Authorised Autodesk Trainer
.
Autodesk Product Design Suite Ultimate 2018
Autocad 2018, Inventor Pro 2018
(personal licensed copy)
.
Johannesburg, South Africa
.
(Impossible only means you haven't
found the solution yet)

[SBix26]

I would rarely use that functionality, but I agree that it should be easier to accomplish and makes your example drawing more readable.

Currently, as you show, one can select Show Hidden Edges for a particular component in a visible-line-only view; the reverse would be useful in a hidden-line view: Hide Hidden Edges.

Sam B

Inventor Professional 2018.2.1
Windows 7 SP1

[Dnyaneshwar_Maid]

Hi I agree with you.

What I thinking is that in such cases can we use combination of BOM - Bill of material keeping part/assembly status as Normal/ reference/phantom with Representations (LOD - Level of detail) in which we can suppressed unwanted part. These setting we will do in .ipt file and while making drawing we will use different setting of drawing view as shown below.

this is a just proposal from my side. As I do not came across any issue where I wanted to show particular edges or lines of particular part. But I always use Level of detail where I can suppress the unwanted part directly which i do not want to show in drawing by defining and selection that LOD

Best regards,

Dnyaneshwar Maid

[rhasell · Accepted solution]

Hi

I do the same as you.

The most frustrating thing is when you show hidden lines for one component but then the entire view shows hidden lines. You then have to change the view to Remove hidden lines, and then start again, by showing hidden lines for one part, then you can hide the lines you don't want. I have also started making a note indicating that some hidden lines have been removed on the view.

One thing is use a lot is "Shift - RMB" and select part priority, and back to "Edge Priority"

The clean-up of hiding individual lines can become quite tiresome, but I have gotten used to it, and much better at selecting how I display things.

Tube ends and break lines are still a sore spot for me, as in your example, you use the defaults, well I have to replace the defaults with custom symbols, now that is a painful task. (Custom symbols will not snap to the cut line of a section break)

@Dnyaneshwar_Maid

Changing the part type to reference in order to manipulate the line style IMHO is a really bad idea.

[MikeKovacik4928]

rhasell

Thanks a million. The changing of edge priority to part priority does what I want and is exactly what I needed!!

What a time saver.

changing part type to reference order is deifinitely not the way to go for doing this particular thing.

Mike

[Anonymous]

---

Can you please kindly confirm is this what you recommended ? ?

> Choosing Edge priority,

> then right clicking on the unwanted hidden line

> and unchecking the visibility option.

[rhasell]

Hi

Alternating between the two to get the best result in order to display the desired information.

Part Priority, will allow you to change the hidden lines for the entire part.

Edge Priority will only affect the selected lines/edges.

Please note that you need to switch back to edge priority once you are done, as most other commands will not work correctly. (I.E balloons, leaders etc)

Hopefully I have answered your question.

[swaveck.keller]

I know this has been solved however.

Option 1

Make the thread boss a separate body and apply hidden lines only to that body.

Option 2

Make the thread boss a seperate part, as it should be then apply hidden lines only to that part,

This will make you Bom structure correct.

Option 3

Use the hidden line calculation in the model tab of the view in the drawing, this requires a weldment I think?

Can someone verify this method as I was trying to use it today, and it was greyed out as I did not have a weldment and was trying to turn of hidden line using this method for only reference object.

Turning off hidden lines manually will cause issues if you make changes latter. 

[rhasell]

Hi

Apologies mate, but I don't understand the problem? Would you mind explaining it again, and if possible, can you provide a screen shot.

And yes, you are correct that manually changing the line display can mess you around a little, but if you are aware of it, it's not as bad as it sounds.

Are you trying to show/ hide lines of a reference object?

If so then you need to change the way the reference parts are displayed.

This might help in this regard:

[swaveck.keller]

Thanks, rhasell, you know how to screen shot, but I want reference hidden line control.

Try all the options in the obvious place (your screen shot dash) and even if show as part, the hidden lines are there reference line hidden visibility.

Here is how I do it manually, select the reference part with part or body priority, select hidden lines.

Next time please read the question carefully and save everyone time.

.Reference Line Manually Hidden

[rhasell]

Hi

Can you re-post the screenshot, it is too small, and I can't see what you are trying to show me.

Thanks.

[swaveck.keller]

I did not mean to be rude, however I already stated I knew bodies and parts in your dashboard.

My question was what is the greyed out bit for.See the bit in the red ELlipse for?

[rhasell]

Hi

Hoping it google translate causing issues. As I mentioned, I did not understand your question, it does not matter how many times I read it, it did not make sense.

Going back, option 2 is the best then you don't want to mess up the BOM in order to change the line style.

As for your last post, the greyed out section is for iParts and iAssemblies. The member list will be displayed for you to select the component you wish to display.

Hope this answers your question. Otherwise, I will continue to try and help.

Regards

[swaveck.keller]

Thankyou, I thought the as mentioned Iparts and Iassemblies was like a BOM reference line selector.

Nope, you have answered my question 100% now.