« ColourLovers: Color for design and more
SolidWorks Gets a New CEO »

Best SolidWorks Dimensioning Tips Contest

Published
by
Josh
on July 10, 2007
in Contests
.

Hello! if you're new here, you may want to subscribe to the SolidSmack RSS feed or to the free email updates. Thanks for visiting!

sandisk-cruzer-2gb.jpg

A few weeks ago I did a post about Dimesioning tips. Looking back at it, I feel it was limited. So, I want to open it up to you and provide a little incentive as well.

I will be giving away this brand new SanDisk 2GB Cruzer Micro USB 2.0 Flash Drive.

To enter the Best SolidWorks Dimensioning Tips Contest, just reply to this post with your best or favorite dimensioning tip. I’ll draw a name next Monday and that person will be 2 gigs more powerful. I’ll accept only one comment from each person, but if you do a blog post with a link back to this post, I’ll count that as a second entry!

Related Posts

If you haven't already, consider subscribing to SolidSmack so you can easily receive updates when new articles are published or announcements are made.

Viewing 18 Comments

    • ^
    • v
    Your "add relations before dimensions" is one of my favorites.

    Here goes with a few of mine:

    *Rather than dimensioning to an edge of a previous feature, use Show Sketch to select the entity that created that edge. That way if you have to add a feature previous to the feature you just created, and that feature eliminated that edge, you won't get a dangling dimension because it was dimension at the source, the other sketch.

    *To reattach a dangling dimension, just drag the leader line to the new, correct entity.

    * Tools-Options-Document Properties-Annotations Display check the "Always display text at the same size" option. This way when you click on a feature to change one of the dimensions, it will display at a readable size no matter what zoom level you're at.

    P.S. My link to your Contest! :)
    <a href="http://www.60hzproductions.com/index.php?option=com_contenttask=viewid=39Itemid=46">http://www.60hzproductions.com/index.php?option...
    • ^
    • v
    My favorite tips (in addition to your solid ideas) include:

    Using the midpoint filter for dimensioning to slots in a drawing.

    Holding the shift key to add a dimension from the edge of a circle instead of the centerpoint.
    • ^
    • v
    Great tips, guys!

    Here's one that I have used quite a bit, but never hear that much about: you can dimension angles with 3 points. The first point selected is the vertex.

    See http://urltea.com/y4r for a video example I did for this tip!

    Brian
    http://cadfanatic.com/
    • ^
    • v
    Awesome tips guys.
    • ^
    • v
    Thanks for putting this contest together Josh. This is an excellent way to get feedback and suggestions for how other users use the software. When I am dimensioning/defining an object I tend to use as many relations I as I can. By adding more relations that usually means that there will be less dimensions that you need to sort through when you need to update something. I use a lot of construction lines to tie features together also trying to eliminate as many dimensions as I can. Thanks again Josh.
    • ^
    • v
    How do I set some dimensions on my drawing with an arrow size that is different from the drawing’s global arrow size?

    The solution to this question requires the use of Dimension Favorites and some preparation.

    Open any drawing that has dimensions. Go to Tools pulldownOptionsDocument Properties tab and select Arrows in the left pane. This will bring up the window with several sections related to Arrow sizes. In the Size section, change the dimensions of the arrow as desired. Pick (left-mouse-button click) OK. This will change the drawing’s arrow size globally.

    Pick any dimension on the drawing. The Dimension Properties pane will appear in the Feature Manager area. SolidWorks has a Favorites section for each dimension. This appears at the top of the Dimension Properties pane. Pick Add or Update a Favorite button. Enter a name in the corresponding window that appears and pick OK.

    Pick the Save a Favorite button. This brings up a file save window. Enter a file name and pick Save. This has now saved the Dimension Favorite for future use by any drawing. Now quit the drawing (do not save the drawing).

    Open up the drawing where the new Dimension Favorite is required. Pick the dimension(s) that will use the new Dimension Favorite. In the Favorites section, pick the Load a Favorite button. Find and pick the desired Dimension Favorite file and pick Open. The Dimension Favorite will now be applied to the chosen dimensions.
    • ^
    • v
    for some reason all the plus symbols got removed... here it is again

    I think the previous Comment is overlooking a huge Tip with using favorites. Tolerancing. If you have a bunch of tolerances that are different than your standard tolerances you can set up whatever type of tolerance you want wether it be an equal bilateral/ unequal bilateral, limits... etc. Set up your plus and minus then save the tolerance. One thing I do is make a bunch, for example plus2-2 plus3-3 plus2-3 plus3-2... and name them just as it is shown, it will save oodles of time.
    • ^
    • v
    My favorite three are:

    1. Take some time and make sure you design intent is captured in the sketches of your features and then take some time and spread out these dimensions so that they'll come in in some sort of position that you need to desrcibe the part.

    2. Use 'Mark Dimensions to be Imported into the Drawing'. When you don't need to see the dimension but require it for feature creation, this works great.

    3. Don't try and completely dimension plastic or cast parts. Use a general note that the CAD data contains dimensions not shown.
    • ^
    • v
    When editing a sketch, double click a dimension to edit it's value, then hit the 'down' arrow key. This will automatically open up the equation editor, create a new equation and insert the dimension name into the new equation. Ready to go. Saves many mouse clicks.

    Arc length dimension - click endpoint of arc, arc itself and then other endpoint. Note however that it wont display correctly with dual units enabled.

    Show sketches temporarily in a drawing to get lot's of free virtual sharps to dimension to.
    • ^
    • v
    Creating virtual sharps:
    Do you ever find that you need to create a virtual sharp in order to dimension to a filleted or chamfered corner?

    Here's a great trick that works in sketch mode and in drawings.

    Control-select the two theoretically intersecting entities (these can be sketch lines or model edges).

    Now simply click on the Sketch Point icon in the sketch toolbar.

    You now have a fully defined sketch point that locates the virtual sharp!

    Behind the scenes, what just took place is the sketch point was inserted with an Intersection relationship with respect to the lines/edges you had preselected.
    • ^
    • v
    Well, the drawing has been held and Steve Calvert will now be able to carry 2GB more stuff around with him. Congrats Steve!!
    • ^
    • v
    Give it to Russel! This is an AWESOME TIP! No more RMB, chooseing min/max arc condition.

    "Russell Jul 10th, 2007 at 12:39 pm

    Holding the shift key to add a dimension from the edge of a circle instead of the centerpoint."
    • ^
    • v
    I know I can't get a USB key (everybody needs one) but I do want to add my 2 cents.

    It is very hard to list the order to do things, but I feel a few good tips are:

    *Fully define as best as possible as you go ( if you do it all at the end you are more likely to just add dimensions that that fully define you sketch and don’t truly capture the intent)
    *Parametric are your friend… the more you use them the better you will be.. so keep using them. All the time, even if you don’t need to, just make it a way of life that way it becomes second nature. Solid Modeling should be like and extension of you hand it is a TOOL to work for you… So learn how to make it….
    *Always Capture you design intent
    *Use symmetry whenever possible
    *Delete that Stupid auto CAD like command the lets you sent the size of an entity without defining it… if you know that size set a smart dimension
    *Setup Shortcut keys so you can Add Smart dimensions as you go ( used “D”)
    *Add fillets and chamfers last unless you want circles or other geometry to be concentric with you fillets
    *keep that origin in the center of you sketch unless you really don’t want in to be… very seldom if there a part that doesn’t have some form of symmetry and So helpful to have those planes in the middle of your part when it comes to later feature and assembly.
    *If you have the choice between a Dimension and a relationship use a Relationship

    Those are a few things that may give you inspiration…. Most importantly… make the computer work for you…

    Al
    • ^
    • v
    Use the ”Hide Line” tool to hide unnecessary things like fillet lines before dimensioning. It will clean up your drawing, make it look better, make it easier to read and make it easier to dimension.
    Randy
    • ^
    • v
    thats awesome!

    dont know how much i can help....

    - you can select the plane or planer face where you want to create your sketch, right click and select create sketch will same 2 mouse clicks.

    - rotation, select the edge and press middle mouse button, now you have a new defined center point.

    -----------------------------------------------------------------------

    ------ question------------

    can anyone help me to figure this out, coz i used to CATIA, and love to swap visibility,

    so, is there any option that i can use to know what are the features that have been hidden in a model.

    (coz, if you mirror more than 2 bodies, and you select one of them to be hidden, you have to keep browsing the specification tree for a particular hidden body..... that takes lot of time) can anyone provide the quick fix for it?
    • ^
    • v
    Hi Everyone..

    I am working on dimensioning a drawing which has fillets and chamfers on round surfaces...Therefore on the 2-d view they are not "true" edges of chamfers or fillets....Is there a good way of dimensioning these types of features on round surfaces?? I hate to create a full section view just to get the true cross section of a small fillet...Or, do I just need to do this ith a manual annotation note?

    Thanks a bunch for any advice...

    Mike
    • ^
    • v
    Hey Mike, sometimes I'll add some sketch entities manually on the views and dimension them. It's probably best to do true section though. If your company allows it you could try to show this in an Iso View or Iso section view. makes it clearer sometimes. you can make a Iso section view by right clicking on the section view and selecting Isometric Section View. hope this helps!
    • ^
    • v
    anybody here know of a good site to find more info on 18 wheeler flash? I\'ve got this site bookmarked and im gonna keep checking it out, but i still would like to find a site that covers 18 wheeler flash a little more thoroughly..thanks

Trackbacks

close Reblog this comment
Powered by Disqus · Learn more
blog comments powered by Disqus