overriding dimension values in drawings

hi,
got a couple questions for 2001:
1. Can anyone tell me how to override dimension values in drawings??? I
tried thru properties but it keeps the original dimension.
2. Also I have a drawing consisting of several assemblies, I want to show
only one assembly with hidden lines and the others as no hidden..... is
this possible and if so how.
3. How do you make x-sections for assemblies, I know how to do it for parts
but there is no option in assemblies...... or is there?
just like to thank everyone for helping me over the last little while, today
is my last day of work before heading back to school and need to finish up a
couple projects.
taker easy
Reply to
Dennis Beifus
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: hi, : got a couple questions for 2001: : 1. Can anyone tell me how to override dimension values in drawings??? I : tried thru properties but it keeps the original dimension. : Shown dimensions (ones you created to define a model feature) can be changed. This will modify the part when drawing/parts regenerated. Created dimensions (ones you created in the drawing with 'Insert>Dimension') may not be modified. These are just a measurement of a linear/diametral distance. They will usually update if you modify the part.
: 2. Also I have a drawing consisting of several assemblies, I want to show : only one assembly with hidden lines and the others as no hidden..... is : this possible and if so how.
Highlight the assembly view you want to change to no hidden lines. RMB Properties, then, from the VIEW MODIFY menu, select View Disp and No hidden. : : 3. How do you make x-sections for assemblies, I know how to do it for parts : but there is no option in assemblies...... or is there?
You need to pick an assembly datum at the highest level of the assembly which you have left unblanked (blank all other datums on datum layers) when you create the section view. : : just like to thank everyone for helping me over the last little while, today : is my last day of work before heading back to school and need to finish up a : couple projects. : : taker easy : :
Reply to
David Janes
: If you want to replace the actual dimensions shown with a value or : symbol of your choosing you can do this to 'created' dims (as opossed to : 'shown' dims) by using the following. : : In the Properties | Dimension Text box you may see the following: : : {0:@D} : : change the 'D' to an 'O' (not zero) and add whatever text string you : want shown: : : {0:@O} 4.500 : @o is actually a note paramter, indicating that, in a multi-line note, the leader should be attached at that line with the @o. Anything following it is also treated as a note, so is not parametric.
: Note that when doing this, no tolerances will show. : : This also work for text: : : {0:@O} MEASURE HERE : : : The actual part dims, if shown on a drawing, cannot be changed in this : manner. : : Out of scale dims used to be called out by underlining. This is a real : pain to do in Pro-E. But now that I look, I can't find a reference for : out of scale dims in ASME/ANSI 14.5 1994, maybe they removed it? : Still in ANSI, but, I believe, they call it something a little different, now. In addition to @o for modifying text, here are some others:
For super-scripted text @+your_text@#
For sub-scripted text @-your_text@#
For boxed text @[your_text]@
For symbolic name of dimension in note @Syour_text
Underlining is handled in 'Properties>Text style' with a check box : : :
Reply to
David Janes
: Since I'm new and haven't even gotten into dimensioning yet, I'm still a : little unclear with this thread. Are you saying that it IS possible to : change created dimensions? : The neat thing about Pro/E is that you have associativity. A dimension available in the part and shown in the drawing can be changed in the drawing and be used to update (regenerate) the part. Main thing to keep in mind: it all starts with the part. Created dimensions do not exist in the part. They are simply a measurement between entities shown in the drawing mode. They are not parametric, meaning, you can not modify them directly. They have no relationship to the part. They may, however, reflect changes you make in part mode; but, they may also lose draft refrences if you, for example, delete a feature or sketcher entitiy referenced by the drawing. Such a dimension is dependent on the part but doesn't interact with it, in other words, is not associative.
Threads are another matter. Created using the hole function, they do not change with the shrink factor added. They are created with a parametric note which is not affected by adding shrink.
: I ask this because I KNOW it will come up in the near future at work. : There's a certain product drawing that we create for the shop to use. We : then make a duplicate of it for the customer, but with the shrink REMOVED. : Using CV, it is VERY easy to modify dimensions by a percentage, or a scale. : For instance we might change the dimension scale by .9978 to remove the : shrink. We do NOT change the actual geometry because we have no use for it : w/o shrink. We simply have two drawing files, one for us and one for the : customer - identical parts, but with two different sets of dimensions. Are : you saying we can NOT do this in Pro/E? Or that we would have to select and : edit each dimension individually? : Well, you've jumped right from the basic, I'm-just-a-novice-user stuff, right into the advanced stuff, no preamble, no buildup, no easing into it, just bang right into the meat of it. Well, here goes. Family tables will allow you to have variations of the same model/assembly, including those with a shrink factor added and one without shrink. Shrink is a parameter which can be referenced in a family table, thus you can have a drawing referencing either of these variations (one for the customer, one for the tool room). This is also not difficult to do in Pro/e ~ much depends on knowing how! Start making a list of the functions you need. Don't worry about how you used to do them. In Pro/e, it won't be anything like that. You're starting all over, from scratch, with a new concept, the concept of the model. The good thing is that it's actually more like making things in the real world.
: Otherwise, the only viable solution is to make another file and scale it : down so it will alter the dimensions accordingly. I know, they used to have : to edit each dimension individually on the boards, but the point of the : computer is accuracy AND speed...isn't it? : : : Da Crew : : : :
: > hi, : > got a couple questions for 2001: : > 1. Can anyone tell me how to override dimension values in drawings??? I : > tried thru properties but it keeps the original dimension. : > : > 2. Also I have a drawing consisting of several assemblies, I want to show : > only one assembly with hidden lines and the others as no hidden..... is : > this possible and if so how. : > : > 3. How do you make x-sections for assemblies, I know how to do it for : parts : > but there is no option in assemblies...... or is there? : > : > just like to thank everyone for helping me over the last little while, : today : > is my last day of work before heading back to school and need to finish up : a : > couple projects. : > : > taker easy : > : > : :
Reply to
David Janes
I think the question was: can I modify the value in a dimension on a drawing?
The answer is Yes for 'created' dimensions only. Created dimensions can loose their references, in which case they show up a violet in color, and you can, in most cases 're-attach' the dimension.
The issue of 'shrink' is a deeper issue.
First, can you create a system of units to use for drawings only? I believe so, but have not tried this. In any system of units, 'shrink' is no different than using 'mm', or 'in'.
Second, The system of units would be associated to the drawing (via a *.dtl file) at drawing creation. Existing drawings can also be modified, but any dimensions created before the new system of units was applied would have to be changed individually.
Third, much easier than changing all of the part features by using family tables, is the concept of 'shrink' as a feature that can be shown on the feature tree and supressed or resumed as needed. Pro-E has this but you must purchase Mold design.
Fourth, I have tried to use extern|copy|geom to reference a new model (with shrink) from the original model (without shrink) and apply a new system of units to 'shrink' this new model. I believe that this works for isotropic shrink, but I have not tested it thouroughly.
/Rant Lastly, Having used CV and Solidworks, I believe that Pro-E is well behind the curve in respect to this feature. Making you purchase Mold design to be able to apply shrink may make sense to the marketing dapartment of PTC, but not to designers like myself who have no need of the features included in mold design (automatic mold selection, etc...), but need shrink. So I do without, for now. Rant/
Just my $0.02
Reply to
Chris Gosnell

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