Continue to Site

Welcome to MCAD Central

Join our MCAD Central community forums, the largest resource for MCAD (Mechanical Computer-Aided Design) professionals, including files, forums, jobs, articles, calendar, and more.

exclude comps from cross section

saspinall

Member
hi


got an assembly drawing in which we show a full cross section but we want to show one of the sub-assemblies in the cross section as a full part ie not sectioned. How do we do it?


Stu
 
Move your cursor over the "hatch" until it highlights. Now right-click and go to properties. You will notice that the hatch for a singlecomponent is highlighted in green. You can now change the "hatch style"for that component. You can change the angle, spacing,Excl Component, or Restore Component. If the Xsec for the component you wish to change is not highlighted, select Next Xsec until to get to the componentyou wish to change.


After excluding components, on the top tool bar select, View, Update, Drawing View and select the view you just changed. The component(s) that you wanted to show "complete" will now be there.
Edited by: appinmi
 
cheers Allan


We got there in the end by going through the components in the hatching properties and excluding them, then going into view > component display and setting the style to Standard of the component we didnt want showing as a section.


Cheers for looking at my post and replying


Stuart
 
Is there any way to 'mark' a file so that it is not cross-hatched by default? Drafting standrads say that hardware/purchased items are not cross-sectioned when they are cut by a section plane. UG has an attribute that can be assigned to the model so that the software knows to not apply hatching to certain parts. Does pro/E have any setting that will allow this?
 
I don't know of any way you can get Pro/E to do that automatically. I also never heard of that convention. What drafting standard are you referring to?
 
iagree with dr_gallup that there is no convention like that toassign some attribute to an assembly to make section of some thingand neglect the rest of the things.


InPro-e what you has to do is already described by allan
 
We have a mapkey to either FILL or EXCLUDE components in our cross-hatching and this is acheived by inserting a Datum Point into the part and re-naming it to either FILL or EXCLUDE. Then when the mapkey is run, it looks for the Datum Point name and either FILLS the cross hatching or excludes the component from being cross-hatched. If there is no Datum Point then the part is cross-hatched normally. If you want to see the mapkey code, drop me a line and I'll email it to you.


Stu
 
ASME Y14.3M-1994, Multiview and Sectiuonal View Drawings


Section 4.3 Non-sectioned Items in the Cutting Plane


4.3.1 Sectioning Assembled Items. Where the cutting pane lies along the longitudinal axis of items such as shafts, bolts, nuts, rods, rivets, keys, pins, screws, ball or roller bearings, gear teeth, spokes, and the like, these parts are not sectioned except where internal construction must be shown.
 
It looks like PTC has a gap in their functionality to support ASME drafting standards. The componenst that are not required to be sectioned should have an attribute set that will allow the crosshatch code to ignore them when encountered.
 
Result of some dabbling ...


2006-08-18_054928_drw_to_pdf.zip


If it's worth investigating the basics amount to putting the solid body on a layer, creating a Copy > Solid Surfs, also on a layer,and then controlling visibility in the drawing using layer visibility.


/ / / / / / / / / /


Nah, never mind. HLR doesn't work correctly on quilts
in section views limiting usefulness to near zilch.
(show_quilt_... no go)


I don't suppose WF3 has added some sort of exclude by
rule function?


Oh, well. On to substitution by envelope or
shrinkwrap. Maybe I'll just have to exclude one object
instead of many.


The build I'm using WF2 M010 also has a bug; random
changes to the assy (or something) cause the excluded
comps to show hatch again and it's necessary to
Restore Comp, Excl Comp every part again. Well, I say
"bug"; possible I'm not doing something according to
plan that causes the problem.

Edited by: jeff4136
 

Sponsor

Articles From 3DCAD World

Back
Top