Automatic Dimensioning

[Adrian2]

Dear Folks;

A couple of questions about Solidworks 2001 dimensioning within drawing files.

I dont get any dimensions automatically showing up in my drawing. So far I have had to place all dimensions manually. Is there a setting I am missing. Automatic dimension insert from model is checked in my options menu.

I also have to place any centermarks and centerlines that I need. Should this also be an automatic procedure ?

Kind Regards

Adrian

 

[meintsi]

After your drawing views are created, use the INSERT - MODEL ITEMS command.

If nothing in your drawing is selected, all dimensions in all views are inserted at once. This can get quite confusing. Sometimes it is more beneficial to highlight a particular view and bring them in one view at a time, but I often use the feature manager tree to bring in selected dimensions into to selected views individually.

But sometimes the dimension you are after will not be inserted into the view you want and then you have to bring them into a different view and use a crtl-drag to copy them to the view you want. (shift-drag will move the dimensions from view to view) On a rare occasion though, this won't work either and your're stuck entering them manually.

Dimensions which are inserted into the drawing which you don't want can be hidden also. The is an option under TOOLS - OPTIONS - SYSTEM OPTIONS - DRAWINGS which will eliminate duplicate dimensions from being inserted.

Icons are available for the toolbars for both the insert modal items command and the hide/show annotations command.

Good Luck.....



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

 

[MadMango]

I'd like to add that the dimensions that are placed in the drawing come directly from the geometry you used to create your model. So if you aren't getting the dims you are looking for, chances are they didn't exist in your model from the begining.

This might sound basic, but I remember an engineer that had a fit with Insert>Model Items>Dimensions a few years ago. He was under the impression that SW would detail the parts for him too. "The attempt and not the deed confounds us."

 

[2Dto3D]

Many of the people I work with prefer to add all of their dimensions at the drawing level, rather than bring them in from the model. They're not interested in driving the model from the drawing, and they feel it's easier than sorting out all the dimensions that come in with the model. Does anyone have opinions or comments to share regarding this? Charley Leonard
CSWP

http://www.2Dto3D.com

 

[BBJT]

Our users are pretty much split down the middle of the road on this. As far as sorting out all the dimensions there are some tricks in doing this.

Insert model items per feature. You can select a feature in the view or drawing tree and import the dimensions just for that feature. This helps minimize the clutter of bringing all the dims in at once. You are also concentrating on the particular feature which should help in making sure that all the dimensions are in the drawing to manufacture that particular feature.
BBJT CSWP

 

[MadMango]

We don't have a set procedure when detailing parts. Some of our users insert as many dims as they can, then delete what they don't want, and add the missing dims manually. When I build parts, I try to put all info (like tolerances) in the model, then insert as much as I can in the drawings. "The attempt and not the deed confounds us."

 

[Timoteo]

Hi guys,

"Split Dimensions" in Drawings are gone. Perhaps the new version of SW made this functin easilly! Wait a little more and the you´ll see "Perfect Dimensions" in drawings.

About the automatic centerlines and centermarks, in SW 2001+ only with API. But, the next version of SW, perhaps...

"SW 2003 is arriving, be ready!!"

 

[Adrian2]

Dear Folks;

Many thanks for your kind assistance. I will make use of your suggestions. The technique of inserting required dimensions on a view by view basis seems to make the most sense for my needs. I do think adding the necessary dimensions is easier than deleting or hiding parametric ones in a large assembly.

I am surprised SW cannot lay down a centerline in a drawing view automatically. It does such a neat and easy job taking sections through things and just about everything else you might want to do.

After creating a professional looking drawing I am left trying to fit a manually drawn centerline which will just end up hanging in mid air if the model position gets changed.

Regards Adrian

 

[brengine]

Adrian,

For centerlines thru cylindrical features:
-First go under the View Menu and turn Temporary Axes on. Then you have to manually Sketch a reference as usual but at least now you have the Temporary Axis line to make your sketch line Collinnear with. I usually add a dimension to each end of the reference line (say, extend 0.25" past each edge of the part). Then delete both dimensions and then "Fix" each end of the line. Lastly turn Temporary Axes off. Certainly not Automatic, but works and stays parametrically linked.

For prismatic parts:
I do a similiar method but use the main (or reference) plane(s) of the part.

For Centermarks:
I found a Macro on the Internet that will place all of them on a selected face in one view (at a time). Usually gets 90% of them...doesn't usually do all incomplete circles so I have to add those where I need them. I don't remember where I got it from so sorry I can't provide a link or give credit, but when I get to work tomorrow I can post it here if you're interested.

Ken

 

[Peva]

Use the insert model dimensions. This way you have more options to do what you want in the drawing. If you don't want to show them, just hide them. The model is the master, and if you don't want detailers to make model changes that can be done on the install of SWX. Remember that you are a designer and all of the design thought (or rules) are put into the model itself. Dimensions, tolerances, GD&T, notes, etc., should all be in the model so that the design intent is present in the model and/or the assembly. The drawing is just a means of showing the design intent on paper. All of the model properties can also be linked notes in the drawing, which can again be shown if you like automatically, and not just added to a drawing. The design intent is in the model/assembly and this is always kept in mind while designing,so why not keep it there.... not the drawing. In other words you can just send the model/assembly to another designer and they can understand the design intent with the drawing.