Warning Construction Geometry Isn't

[ongybill]

Just a note so others don't have the same problem I ran into yesterday.

After getting far into a complex cabinet assy I found that the 19" rack mount section was the wrong size.

Traced it down to some reference lines. Turns out that all CONSTRUCTION GEOMETRY is in centerline format (not changeable as far as I could find). So, when I dimensioned other lines from the construction lines it introduced a midpoint relationship so that when I typed in 1.75" spacing, it actually spaced the new lines at .875".

Big cabinet, and until I zoomed in later I couldn't tell that the dimension was not between the 2 lines as I thought, but between the line and a point in space 1/2 way beyond the construction line.

This was for the 2nd of many features added to the cabinet. By the time I moved all the child features to where they should have been in the first place I ended up with a model with 12 solid bodies instead of 1.

Anyway, just a friendly warning. Construction Geometry isn't really just "reference geometry" like with most software. It's a centerline, and there may be hidden relationships (ie diameter dimensioning) that you're not aware of and are undesirable, so be careful.

 

[Heckler]

I use planes to define critical interfaces. I'm assumming this cabinet is designed IAW EIA-310? I believe (I haven't looked at that spec in over a year) that they define interface planes so you can use those instead of converting a line to construction geometry. Just a thought.

Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 4.0 & Pro/E 2001
Dell Precision 370
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"There is no trouble so great or grave that cannot be much diminished by a nice cup of tea" Bernard-Paul Heroux

 

[Theophilus]

Right. Heckler was also on to something regarding the conversion of construction geometry to lines and vice versa. There is a sketch tool button that toggles selections between the two (otherwise, how would you construct a circle in construction geometry?). I use this all the time.

I also deliberately use the construction geometry as a centerline for dimensions. It's strange to dimension a radius of something with a diameter of 0.375"--especially when you create this as a revolve where all the geometry is to one side of a centerline. So this action as a centerline is useful unless you're not expecting its effect.


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[CorBlimeyLimey]

ongybill ... when placing a dimension from a normal line and a construction line, you have two options when clicking where you you want the actual text to be placed.

1) Clicking between the two lines will give a direct distance between them.
2) Clicking on the side of the construction line away from the solid line, will create a "doubled" dimension. This is suitable when using the sketch to create a revolved feature. When the dimension is inserted into a drawing view, it comes in as a diameter.


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[smcadman]

There is a sketch tool button that toggles selections between the two (otherwise, how would you construct a circle in construction geometry?).

After drawing sketch entities, such as lines, circles, arcs, etc., there is a check-box in the Task Pane "For Construction". (if the item is not already highlighted, highlight it first)

Flores

 

[SBaugh]

Traced it down to some reference lines. Turns out that all CONSTRUCTION GEOMETRY is in centerline format (not changeable as far as I could find)

There is an icon that allows you to change a Construction line to sketch line and back. Look under your Sketch tools toolbar, for the icon. I would post image, but I don't have access anymore.

This is also in the help listed as Construction geometry. "When in doubt use the help"

Anytime you are in a sketch or you make other sketches after another one and you use points, lines, Construction geometry (centerlines) etc... then you will have child relationships and you need to be aware that this happens.

Most users I believe understand this concept.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

faq731-376

 

[ongybill]

{So this action as a centerline is useful unless you're not expecting its effect.}

I'd find it more useful to be able to create ACTUAL construction lines. If I WANT a centerline, I'll draw a centerline.

I WANTED 'construction geometry'. You know lines that showed me where the edges of the cabinet were even when the solid bodies were hidden, but didn't do ANYTHING else. Reference Geometry (not centerlines). I'll NEVER want a diameter relationship when drawing a rectangular box, or on reference lines I use to show where interior components or mounting surfaces are.

What I got was interactive geometry that DID do something else, and WASN'T 'construction geometry', regaurdless of what it's called.

Since this isn't documented in the help section, I'd call it a bug. (Sorry old joke: What's the difference between a feature and a bug? A feature is documented).

 

[CorBlimeyLimey]

You will have a more stable model if you use reference planes or at least layout/skeleton sketches to drive your model.
A layout sketch is only used to create converted entities in other sketches ... never directly with a feature.
This way you will place a centreline (albeit still a construction line) only where & when you want, for use with a feature. A construction line in a layout sketch does not allow its use as a centreline in another sketch.


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[ongybill]

Like I said just a friendly warning. SOLID WORKS DOES NOT HAVE TRUE CONSTRUCTION GEOMETRY. I know I'm not the only one that's unaware of this.

You can draw solid lines, or you can draw centerlines. You can convert them back and forth with the touch of A button, but you CANNOT draw construction lines, so be CAREFUL.

I hope this tip saves someone else from messing their models up.

 

[ctopher]

For parametric CAD (solids), there really is not a need for construction lines. There are tricks, like creating a sketch by itself to use as construction geometry. For parametric you create the sketch then extrude, cut, etc without the use of const lines. I don't see this as a problem for the majority of SW users.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP3.1 / PDMWorks 05
ctopher's home site (updated 06-21-05)
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[Theophilus]

If you take CorBlimeyLimey's advice, you'll be greatly ahead in using SolidWorks to its potential--especially regarding the capacity to quickly edit lots of geometry in your model.

The centerline is construction geometry unless you otherwise use it as a centerline. This cuts down on feature and toolbar clutter simply by knowing under which conditions a given line is construction geometry (completely benign) or a centerline (acting as an axis for a dimension, sketch, or feature). Perhaps we could request an enhancement that would automatically denote when construction geometry is being used as a centerline--different dash pattern, color, whatever.


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[aamoroso]

The line doesn't become a centerline until you create the dimension as a diameter.

Fill what's empty. Empty what's full. And scratch where it itches.

 

[smcadman]

Just be glad you didn't get the standard speach:

"Forget everything you learned using ___________ (fill in the blank, usually AutoCAD), this is Solidworks"

(You will find it a few dozen times on here)

Flores

 

[Theophilus]

Forget everything you learned using AutoCAD, this is SolidWorks.


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[meintsi]

lmao......

ongybill,

It seems that what you want would be called a layout sketch. Create a sketch of what you want to see, and close it without using it to create a feature.

Move to the top of the tree and you will see it ALL the time until you choose to hide it.

Remember...
[navy]"If you don't use your head,[/navy]
[navy]your going to have to use your feet."[/navy]

 

[ongybill]

Thanks for the tip on the layout sketch.

Actually, now that I know to be careful with the pretend construction lines I shouldn't have any more problems. If I ever reference from one again I'll make VERY sure it dimensions properlly.

I have found that it's very useful to use construction lines to show where something inside a complex assy or part is. Particularly if I'm going to hide the solids while sketching.

While in sketch mode rotate around so you can see the location of an interior mounting surface for example. Select it and convert the edges, then change them to construction lines. When you convert the edges SW puts lines on the plane you're sketching on that are aligned with the interior surface/feature/part. Now if you hide things you still know where they are. Very useful feature.

Just something I find useful, perhaps some other newbies will as well.