Parametric Dimensioning

[D3sign3r]

Ok hopefully sw can for sure do this.
If im detailing a simple recangle plate, in sw2003, and i place a hole in the center, how do i specify that that hole will always be in the center of the width of the plate? Even when i want to change the width dimension later on? The Dimension modify box wont allow me to enter in the width name "D1", which i would like to specify "D1/2"...
thx.

 

[ctopher]

see FAQ559-758

 

[macPT]

You can use Tools/Equations to add relations between dimensions.

Regards

 

[Mandrake22]

To expand on the previous responses:
1. Sketch a construction line from corner to corner.
2. Right click this line and select "midpoint".
3. Control select the center point of your circle sketch.
4. Create a coincident relation between these two selected points.

 

[MechEng13]

To Expand on Mandrake

You can

1. Select the Construction line
2. Select the Center Point of the circle
3. Add a midpoint relation to the 2 selections.

One fewer step.



Alan M. Etzkorn
Manufacturing Engineer
Hoffco/Comet Industries Inc.

http://www.hoffcocomet.com

 

[ctopher]

You can get by without a construction line from corner to corner....ctrl select midpoint of each horiz and vert line of the rectangle and the origin (located in the middle of the part) and make them coincident.

 

[TheTick]

-OR-
draw construction line, then constrain symmetric to one pair of edges. Constrain the hole to the construction line

All this machinery making modern music can still be open-hearted.

 

[D3sign3r]

Yeah that method worked,mandrake22. Now how do i use the Equation method? Im entering in D1@Sketch1 / 2 but im getting an "equation entered is invalid" error every time. I cant seem to get much info out of the 'help' file in SW.
thx.

 

[Arlin]

You need to add/eddit equations by goint to tools->equations.

You cannot simply type an equation using dimension names in a dimension modify box (Like Inventor).

 

[macPT]

You should have something like: D2@Sketch1=D1@Sketch1/2.
If you don't know the dimensions name or don't want the trouble of write their long names, just click on the dimension when you are editing the equation: SW will write it for you. Then just add the needed math functions.

Regards

 

[brengine]

I wouldn't use equations. They're not real reliable. Instead, try to constrain it with some construction geometry if you can.

Ken

 

[Regg]

The variable names have to be enclosed by double quotes: "D2@Sketch1" = "D1@Sketch1"/2

While I have not found equations to be unreliable (yet), I would first use construction geometry (preferrable) or relations. They show up first when you edit the sketch.

Regg

 

[dgiy]

Ken,

Can you give me an example of when equations are not reliable in solidworks. I use them from time-to-time and want to know when not to use them. Or maybe you meant that the user may not use them reliably??

Can you clarify please.

Thanks,
DG

 

[TheTick]

Addresses one possible trap related to equations:

faq559-590

 

[brengine]

dgiy,
My last and worst experience with equations was this (running SW2001 at the time I believe). In my main assembly, I was using equations between multiple parts and sub-assemblies. It was a ball feeder, and I wanted multiple parts to update when the inputted diameter of my ball part file was changed (i.e. hole sizes to update, plate thicknesses, and mates/relations between parts, etc.). There were occasions when the equations were *not* updating the parts, some equations were wrong and I don’t think I saw any notification that they were wrong, and then having to manually update the filename in each equation (if a part or assembly filename changed) was a mess. Once I had this assembly completely working, later I copied the assembly and all it components, then tried to change the ball diameter and let SW work all it’s magic (thinking I wouldn’t have to do any work). It was a nightmare. Some files were looking at the previous assembly base ball part, and some files in the previous assembly were looking at files in the new assembly (which was probably *not* a fault of equations tho, but I still wonder). And all of the equations still contained the old filenames in them. A year and 3 or 4 more times coping this assembly later (with a day or 2 of headaches), I decided to delete all the equations and the base ball.sldprt file. I then created a layout sketch in the main assembly, and had all my (previous equation) references point to that construction geometry. I’ve only copied it once since then for a new ball size, but that time was much smoother.

At that I time I was advised that equations were quirking and not reliable, and to avoid them if at all possible. I haven’t used one since then.

I would think that only using them inside a single *part* file (not looking at *any* other files), and not a really complex part shouldn’t cause any of the problems I saw, but I haven’t seen the need to use and equation (for simple add/subtract/multiply type equations) that couldn’t be done with geometry...so I do it with geometry. In these files, if there are going to need to be multiple relations, I usually have a layout sketch *only* as the top most entry in my feature tree. All that’s in that sketch are my “equation” geometry lines/arcs/circles that subsequent features will look at. For just one or 2 relations, here and there, I just put the construction geometry in that respective feature’s sketch.

Also, most of my work is 2-1/2-D (rectangular/shaft) type parts, no curvy stuff.

And before I get flamed, I know there are times when equations are the obvious, and best way to go, but I choose to go the another way. Just take a look at

http://www.mikejwilson.com

and see what he did with equations. Another good thing I could say is that I do like the fact that equations now show up in the feature tree. That makes it easier for another user (or me later down the road) to notice that they actually exist in this file and are being used (I don’t think that was in there before).

I’ll try to keep an eye out for a good instance to use one and maybe I’ll dip my feet in there again...maybe...;o)

Just my $0.02,
Ken

 

[brengine]

dgiy,
And yes, I *was* a much greener designer at the time and may have been throwing the equations around were they weren't *really* necessary. I would definitely not go overboard with them (just like in-context relations). But they still failed in my opinion.
Ken

 

[brengine]

dgiy,
And I do as the tip that TheTick recommended, I also rename the dimensions in my layout sketch to be names with real meaning, not just Sketch1 and Sketch2, blah.blah.blah.
Ken

 

[macPT]

Ken
About equations I've never experienced problems but, as you say, I only use them inside parts (not relating differnt parts).

About the copy of files, yes, I was already in big trouble. I gess SW remembers the place of the original files. You may call the copy assembly, but SW will retrieve the original parts and these are the ones that are about to be modified.

The only safe way that I have found to do this is by changing the file location option of SW, to point only to the intended folder (containing the copied files).

Regards

 

[dgiy]

Not trying to flame you just trying to learn and understand.

Thanks for the heads-up.

DG

 

[Rocko]

KenBolen,
I went to mikejwilsons site they you mentioned and that scooby doo model was very impressive on its use of surfacing. I am curious how long he worked on that?