Creating Dimensions

[kman23]

<DIV>Here's what i am trying to achieve.</DIV>
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<DIV>I have a"L" Bracketto which i will be adding multiple holesor slots on the horizontal or the vertical part of the bracket. The dimension of the L bracket, number of holes and their locationare controlled byreading a data file from pro program. The 3D modelworks really well andI can control all aspects of the bracket accordingly.</DIV>
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<DIV>The problem I have is with dimensioning the drawing. As the holes appear and disappear dependingon the product, the dimensions need to be matched. Auto dimension is to messy and creates more problem.</DIV>
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<DIV>Here is what i have done currently.</DIV>
<DIV>1. I have created all the dimensions that the part can have. </DIV>
<DIV>2. Added groups of dimensions to certain layers.</DIV>
<DIV>3. After I update the drawing, I hidecertain layers in which the dimensions have turned purple because their features have been suppressed.</DIV>
<DIV>4. However, i have to do this every time the drawing changes, also i have to go through the laborious task of creating every possible combination of the dimension and grouping them into layers.</DIV>
<DIV>5. I have tried using drawing states, however Iwill have to create far to many states to make the mode / drawing work. It would be simpler to unhide 10 out of 20 layers automatically.</DIV>
<DIV>6. As an example, if hole1 is present, display dim1. If hole2 is present display dim2. If hole1 and hole2 is present display dim3. I have about 16 holes / slots and they can appear in many combinations.</DIV>
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<DIV>My questions are.</DIV>
<DIV>1. Is there a better way to do what i need to achieve?</DIV>
<DIV>2. Is there a way to hide / unhide layers programmatically?</DIV>
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<DIV>3. How to create dimensions on the fly in drawing?</DIV></DIV>
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<DIV>Please advice.</DIV>
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<DIV>Regards,</DIV>

 

[magneplanar]

kman23,

It sounds like you need "pro-program" so you can write the details into the drawing that will show or not show the features and dimensions depending on the 3d model

check it out...

cheers,

M

 

[dr_gallup]

I would use shown dimensions rather than created dimensions. Then when you suppress a feature the dimensions just disappear instead of turning purple. Resume the feature & the dimensions come back right where they were. If you also use snap lines to control the position of dimensions everything will stay lined up when the part envelope changes.

We ALWAYS use shown dimensions if at all possible. It takes a little work up front to plan the correct dimensioning scheme but I think it is well worth it. Many will disagree.

 

[kman23]

dr_gallup,


You are correct. Showdimension works best and the dimensiondo disappear when the feature has been suppressed. However you have to be a little careful.


I have WF3.0 and I created a sketch for a hole with proper dimensions and an extrude cut to create the hole. Now in the drawing mode I used show dimensions to display the dimensions as I want. Nowin the part modewhen I suppress the extrude, the whole disappears, however the dimension remain in place in the drawing more. It took me a while to realize why and that's why this post. It seems logical now, but what ihave to do is suppress the sketch for the hole in part mode, which will suppress the hole and then the dimensions will disappear in the drawing. Unsuppressed the hole sketch and the hole extrude in part mode, the dimensions comes back just as i had set it up. works perfect!!!


Thanks for all the help and hope this helps some one else.


Regards,

 

[dr_gallup]

That's why I always use sketches internal to the feature if possible. That's the way Pro/E started and it makes much more sense to me than separate sketch features. I don't care HOW solidworks does it.