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Hello Everyone,

 

My name is Tamas, first year engineering student. I'm struggling to replicate this drawing for my assignment.. I started it, but I got stuck with the views. I used a broken-out section view for the top one, but it cut into the screws too, even though I clicked on "exclude fasteners". How can I fix this problem?
Also, how can I create that view above part 2.?
Assignment 2 drawings.30.pdf - Google Drive


Thanks for your help in advance.
Tamas


Categories: Drawings and Detailing

Comments
Last comment By: Tom Helsley   Wed, 22 Mar 2017 18:55:04 GMT
Re: How to create this particular assembly drawing?

Your fastener models need to have the isFastener property set to 1 in the custom properties for the exclude fasteners function to work.  You can always tell SW what parts to include/exclude from section views manually in the section properties dialog box.

By: Meredith Lewis  Mon, 20 Mar 2017 12:11:10 GMT
Re: How to create this particular assembly drawing?

Thank you for that. It worked.
How can I create that view in the big red circle?
Also I would like to make visible that "support hole" in the small red circles. If I click on the component and choose "show hidden edges", it will show lots of other lines that I don't want to be visible. Any idea?
SOLID.jpg

By: Tamas Lanci  Mon, 20 Mar 2017 20:50:24 GMT
Re: How to create this particular assembly drawing?

Ahhh, that's one of the few areas where manually-drawn drawings/views still have an advantage over projected, model-driven CAD views.  That exercise has been in the book since the vellum and pencil days.

 

The closest you'll get for the big oval highlighted area is a partial section taken in the auxiliary orientation and show only the cut surface.  I hope your instructor doesn't expect you to duplicate those views.

 

For the center-drilled hole in the small circled area, you can use the broken-out section tool in the "top" view.

 

BTW, what edition of "Technical Drawing" did this exercise come from?

By: Tom Helsley  Mon, 20 Mar 2017 21:56:59 GMT
Re: How to create this particular assembly drawing?

I did an auxiliary view then a crropped view of that. That is the closest I could get:SOLID.jpg

As you can see the bottom line is not touching the bottom edge of the aux. view. Unfortunately, we have to replicate this drawing exactly.
This drawing is from the 12th edition.

By: Tamas Lanci  Mon, 20 Mar 2017 23:05:01 GMT
Re: How to create this particular assembly drawing?

See my answer below....use a sketch in the 3d to create the aux view in the 2d.

By: Dan Pihlaja  Tue, 21 Mar 2017 13:02:46 GMT
Re: How to create this particular assembly drawing?

To show the little hole, use the shape above for your broken out section.

As for the little view in the top left corner right corner, create a sketch line that is perpendicular to the edge on the fin of the wing.   Then use the sketch line to create the aux view (see example below).  Then you are going to have to crop the aux view.

Then hide the sketch again.

By: Dan Pihlaja  Tue, 21 Mar 2017 13:01:51 GMT
Re: How to create this particular assembly drawing?

Cropping the auxiliary view will work, but other lines may appear.  It looks like your projection lines are not parallel to each other.  Your auxiliary view should use a line perpendicular to the bottom projection line that you drew, not the top one.

 

The views in the exercises are generally crammed with enough detail so you can re-draw the parts, and aren't necessarily intended for the views and dimension placement to be duplicated.  The book explains that at the end of the chapter, where the exercises begin.  Sometimes, the views shown in the exercises do things that parametric CAD just doesn't allow.  Remember, the exercises in that book were created BC (Before Computers).  Try your best, but you may have to find alternative methods in some cases.

By: Tom Helsley  Tue, 21 Mar 2017 17:12:16 GMT
Re: How to create this particular assembly drawing?

Thank you guys. I used Dan's method and it worked I'm getting somewhere now. I drawn an auxiliary view then hid most of the lines around the part, then did a crop view. I would like to remove that sketch that I used for the cropped view(green arrow). Is there any way to do that?
Also, how can I make visible the circled lines(the key and the hole on the clamp screw)?
By the way, I tried to use another broken section view for the support hole, but it didn't work. The the section views interfere with eachother, If I tick "exclude fastener" in the broken section 1., it will apply it to the broken section view 2. too and vice versa.

 

solid.png

By: Tamas Lanci  Tue, 21 Mar 2017 20:19:41 GMT
Re: How to create this particular assembly drawing?

I'm glad to hear your making progress, Tamas.

 

Usually, when you complete the crop command, the crop lines disappear.  When you edit an existing crop, the lines will re-appear until you exit the edit crop sketch.  Try editing the crop sketch and see if other lines appear.  Maybe you have duplicate lines and the second set can just be deleted.

 

As to showing the hidden lines in only the regions you circled, well that's a limitation of SolidWorks.  Unfortunately, you cannot turn on hidden lines, add a broken-out section and expect the hidden lines in the sectioned areas to disappear.  Hidden lines is an all-or-none deal for each view.  This is one of the constraints I was hinting about in my earlier post.

By: Tom Helsley  Tue, 21 Mar 2017 22:44:32 GMT
Re: How to create this particular assembly drawing?

This is not actually true Tom Helsley.   (at least for SW 2015 and forward...I think it was available in SW 2014 as well if I remember correctly) See below:

You can show hidden edges in each view for each feature if you want.

By: Dan Pihlaja  Wed, 22 Mar 2017 12:45:30 GMT
Re: How to create this particular assembly drawing?

Oh, cool!  Funny, After all these years, I never thought of trying individual features before.  I'll have to give that a try.  Thanks, Dan.

By: Tom Helsley  Wed, 22 Mar 2017 18:55:04 GMT
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