Hide section view reference cut lines 1

[jlcochran1]

Is there anyway to hide the section view cut line in SW 2006? In standard pressure vessle detailing each nozzle is simply labeled "DETAIL NOZZLE A" etc. The drawing is not cluttered with section cut lines for each nozzle. It would not be uncommon to have over 100 section views to get all required details. Currently a work around is to create extra views off the paper to cut the scetion and drag the view to the drawing. This is time consuming. In Inventor there is simply a switch to hide the section cut line and/or section label. I have found nothing similar in SW. Without getting into a debate about standards (PV's and tanks have been detailed in the same manner for decades and our customer specifications for the required ACAD drawing format are not likely to change anytime soon) are there any easier work arounds? For example could layers be used and somehow hidden prior to plot similar to AutoCAD? Any ideas appreciated.

 

[ctopher]

In SW, usually you can right-click on a line or edge and select "hide". I have not tried it on a section line.
My 2 cents? Create dwgs per real standards, not ACAD standards.
Look in SW Help. Yes, you can use layers.

Chris
Systems Analyst, I.S.
SolidWorks 06 4.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 06-21-05)

 

[dgowans]

ctopher,

No offense intended, because your input in the SWX and GD&T forums has been and continues to be extremely valuable, but the OP specifically asked not to get into a discussion of standards.

That being said, I will offer the following (rhetorical) question:

If jlcochran1 always makes drawings to the letter of whatever standard (ASME, ISO, etc.) is deemed appropriate, but they are not to the customer's liking/standards, what is the probability of continuing business with said customer?

As I said, this question is rhetorical because I have no intention of continuing this discussion in this thread - apologies to jlcochran1 for the slight hijack......

 

[SBaugh]

Will I tested this, and you cannot hide a section line and the simple reason is because it's not proper standard.

So what you are doing now, is probably the only way you are going to get around this issue.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

faq731-376

 

[smcadman]

For example could layers be used and somehow hidden prior to plot similar to AutoCAD? Any ideas appreciated.

Before we jump on ctopher, jlcochran1 should have tried layers before posting. Putting section lines on layers and turning that layer off is the only way to do it.

Flores
SW06 SP4.1

 

[jlcochran1]

smcadman were you able to successfully get the layer option to work? When I freeze or hide a layer the cut line hides, but the arrows and label remain unless I am missing something, don't work with layers a lot. Were you able to somehow hide those as well? From what I can tell Scott is correct, currently no better work around than pulling extra views off drawing in SW or using Inventor to detail.

 

[ctopher]

dgowans, I know, it was just my 2 cents. Sorry.
I did not want to get into the standards discussion.
Thanks.
I tried changing the section line to a new layer, then turned off the layer. Section line gone.


Chris
Systems Analyst, I.S.
SolidWorks 06 4.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 06-21-05)

 

[jlcochran1]

O.K. think I found a workable solution for now. By putting cut lines on a specific layer and hiding I can get rid of the cut line. By changing the section arrow dimensions to 0 in Tools/Options/Document Properties/Arrows I can get rid of section arrows. The label can be eliminated in the section view property box. Thanks for all the input.

 

[GTCadGuy]

I tried this out, and I created the section (A-A), created a layer and added the section line to that layer. Once I turned off the layer, the section line cut and arrows were turned off. The resultant section cut still was labeled "section A-A". That label can also be added to layer and turned off as well.

Hope this helps.

SolidWorks 2006 - SP3.0
UG NX3
Pro/Engineer Wildfire 2.0

 

[smcadman]

Turn the Layer toolbar on. On the Layer toolbar, pick the box icon or whatever it is and pick the NEW button, and enter Section view for the name. Next, CTRL + pick all of the section views on that sheet and pick the Section View layer. When you're ready to hide the layers, pick the box icon and then pick the light bulb so it is off (white instead of yellow).

Flores
SW06 SP4.1

 

[dgowans]

ctopher,

No problem. It wasn't my intention to bash you by any means. You've proven once again that your input is very valuable by providing a solution to the initial problem.

I think we've all seen a ton of threads get WAYYYYYY off topic without any resolution to the original question and was trying to head that off. This forum continues to be my best avenue to get SWX questions answered and I would hate to jeopardize that by discouraging responses with postings of my own.

 

[jlcochran1]

O.K. thanks, by moving section line after created to new layer vs drawing sketch line first on new layer I can duplicate your results. This will be tremendous time saver.