9 Replies Latest reply on May 5, 2014 7:33 PM by Jamil Snead

# Descriptive Geometry -- How do you get the auxiliary view you want?

I'm working on a project, honing up on my solidworks skills.  I let you follow along from scratch. I'm wanting to build a large quantity of tapered pedestal machinery stands (Vise, Grinder, Swag-off Road Band Saw Table).  In all I need to make five or six of these. So I designed one up with a simple plywood design.  The simple plywood design looks good but rather difficult and very time consuming to glue up. (See photo of temporary blocks glued in place on paper.)

So I saw an alternative construction technique (Shopnotes Issue #97, pg 18 -- If you've never seen this magazine, there are some great projects in there.  I recommend them highly.)  This technique was used on a large cabinet / box structure with vertical sides.

I want to use this technique on a tapered box.  I sketch it up using weldments and a few cuts with surface.  That went smooth. When I go to perform the complete drawing details, I have a major problem pulling off auxiliary views on the index 'leg'.  I spent hours trying to get an auxiliary view to take off.  I could not get view A to pull off correctly.  I finally added a phony element perpendicular to the leg's axis.  Then I was able to pull off auxiliary views so I could do the take off I needed. (And yes I know how to hide the phony element once the aux views are complete.   I left the phony element visible to remind me of how I did this, and to validate View C as TSS - True Size and Shape. )

So here are my questions:

--How do you guys create auxiliary views when the system seems to be fighting you?  Do you create phony elements too?  Is there a better technique?

--If not 2D style descriptive geometry take offs is the a better way to communicate the end view profile, overall lengths and angle cuts of those support elements? (Yes , I know I can do a 3d measure, and write that down on a piece of paper, is that really a best practice?)

--What happened to my butchered View Arrow for view B?  (I've tried every thing to fix that.. its just way too short to be visible.)

Apologies if this question seems long winded.. I wanted you to get into the context...  Many thanks,

LB

• ###### Re: Descriptive Geometry -- How do you get the auxiliary view you want?

Is there a reason you are trying to show all 4 legs in the same view? I think your main problem is that your starting view is not perpendicular to the leg, so then the auxiliary view A doesn't look straight at the end. If you do a view of just one leg at a time you can show it flat (like your view D) and then do the end view off of that. Plus that is better for dimensioning the length too.

• ###### Re: Descriptive Geometry -- How do you get the auxiliary view you want?

Jamil,

Thanks for your reply.  Hmmm.. I do see where I can store my part 'assembly' file (.SLDPRT) with one leg "normal to" the screen. Select a surface, select "normal to" and then save the file with that view.  I can see there is an option to use the "current model view" when creating a Model View in the .SLDDRW file.  It skews at an odd angle, but I can see that does save two or three auxiliary views from my original drawing above.  It definitely fixes the issue for which I had to create the phony element.

This does give me the opportunity to continue to store all of my invidual components within the single weldment part file into a single output file.  I've been testing this, and wow... I can even use multiple weird oriented components.  I choose an element's plane, make it "normal to" the screen, save the file, create a sheet on the SLDDRW file, and repeat.  The system doesn't update the views every time you save the file... once the Model View is created it stays stable, no matter which part viewing angle is stored.

Is that what you are talking about?

Your comment does raise a couple of questions for me... when you do weldments, do you create a seperate .SLDDRW file for each component type, or do you keep them all in one file perhaps on seperate sheets (which matches the file name for the .SLDPRT) ??   At first glance, one prt file and one drw file seems a lot easier to keep track of.

And if you ever did have the need to create an auxiliary view in an odd angle, how would you do that?  (e.g.   I want to see what the assembly looks like from a 3d angle of x,y,z steradians...)

Again, thanks.  LBC

• ###### Re: Descriptive Geometry -- How do you get the auxiliary view you want?

To answer a couple of your questions (I think) click on a surface, as you said, then while holding down Ctrl select another surface that's perpendicular to the first surface.  Then select "Normal to".  That will rotate your model so that the first surface selected is normal to the screen and the second surface selected is at top.  Next hit your spacebar.  That will bring up a dialog box where you can save this view (one of the icons at top) and give it a name.  You can then use this view when placing drawing views in your drawing.  Also while placing this drawing view (or after placing it) you can click the button for "Select bodies" in the drawing view's PropertyManager.  That will take you back to the part model where you can select which body or bodies you want to show in this particular drawing view.

• ###### Re: Descriptive Geometry -- How do you get the auxiliary view you want?

I actually almost never do weldments so I can't help you on best practices there. But as far as doing view at a weird angle, its always pretty much by rotating the part or assembly to the view you want and either create the view right then with "current model view" or even better is to save the view as J. Mather showed. Saving the view is nice because after that if you hit spacebar when you are looking at the part it will list the view there so you can click on it to go back to that view. And if you are inserting a new view on a drawing your named view will show up in the list along with the standard views. That is the only way I know of to change an existing view to a new orientation too, since you can only do "current model view" on a new view.

• ###### Re: Descriptive Geometry -- How do you get the auxiliary view you want?

Normal To (there are a couple of tricks with these to get aligned exactly how you want)

and

Named Views might be of use.

Create the views in part or assembly file and then reference them in drawing file.

• ###### Re: Descriptive Geometry -- How do you get the auxiliary view you want?

In your model, select the large flat face of your leg and rotate your view Normal To that face.  Then go to your drawing and insert a view using the "Current Model View" option.  Use "Select Bodies" to show only the selected leg.  This should give you a view similar to "D", which can then be sectioned/projected as needed for detailing.

• ###### Re: Descriptive Geometry -- How do you get the auxiliary view you want?

Look in the archive of this forum under the heading WYSIWYG Drawings.

• ###### Re: Descriptive Geometry -- How do you get the auxiliary view you want?

Wow.  You guys rock.  Quick answers.  Unexpectedly quick answers.  So now the dilemma.. Can I choose multiple Correct Answers?  Obviously, I first saw Jamil's response and it took me exactly one hour and nine minutes to figure out what he was talking about, play with it, test three or four different times and write a response.  And yeah, I took my time writing the response, thinking other new guys might get stuck here...

Patrick, your answer would have saved me 30 minutes of my life, had I seen it first.   You exactly nailed my experience level and wrote to that level, so I gotta call it.

Jamil, J., Patrick, John and Glenn, many thanks.  And Glenn, that view orientation spin control button trick.. is that documented anywhere?  How would a new guy ever figure that one out?

Again, thanks to all,

LBC

• ###### Re: Descriptive Geometry -- How do you get the auxiliary view you want?

Lb Corney wrote:

And Glenn, that view orientation spin control button trick.. is that documented anywhere?  I don't know.

How would a new guy ever figure that one out?  The same way you and I did, right here on the Forum.