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Numbering The Dimensions In Drawings

tony-ontario

New member
Solidworks Drawing Dimension numbering
Hello everybody, I am a young Toronto based mechanical designer working for a casting company. I am trying to find information on how to number critical dimensions in an automated fashion. Ideally I would like an option that I can choose several dimensions on a drawing, and they would automatically be numbered 1 to 30…etc., and when one is deleted, the number is not reused. I would be using this for our foundry to be able to easily convey the message of what critical dimension they are talking about over the phone, and to use a list of the dimension #’s for inspection documentation. We are currently numbering them with ‘notes’ individually. Aside from the labour, another problem with our current form is that the notes aren’t attached to the dimensions, as that is far too much work for us SW guys, and that when a dimension is moved, you have to manually move the note along with it. We are currently using 2007, but will probably be updating to 2008.

Any suggestions would be appreciated. Thanks for any help to a newbie like me,

Tony-Ontario
Toronto, Ontario
 

ttraser

New member
Numbering the Dimensions In Drawings

Throughout the 25+ years that I've been in the business, I've allways utilized the "zones" on the format for referencing dimensions, changes, etc. I've never heard of numbering the dimensions. However, you are able to show the properties of the dimension which has a numeric value added to it, i.e. d1, d2, d3, etc. You might try to show these on your drawings and utilize it to accomplish what you are trying to do.

good luck, :)
 

Ody_Mech_Engr

New member
I agree zones, using letters in the vertical and numbers in the horizontal are the way to go. Simply refer to the 1.53mm dimension in zone B5 when identifying the specific dimension in question. I've worked with some very complex multi-sheet assemblies that effectively used this and save a bunch of time. The only time I would ever consider giving a specific identifier to a dimension would be if it was highly critical and very confusing. Even then I'd be VERY reluctant.
 

tony-ontario

New member
Thank you both Ody_Mech_Engr, and ttraser for your input, this is a very probable solution for what i am trying to do. I know how to use the grid feature and all, but how would you go about inserting the B5, C7, etc.? In the template, or is there a way to do it rite inside the grid? Thanks again.
 

gwinslow

New member
You could continue your current method and begin attaching (grouping) the notes to the dimensions.
Use control key to select note & dimension, then right-mouse button>group>group. This will keep them together if moved.
 

Zevel

New member
Hi Tony
When you click on the dimension you will see in the "dimension text" box something like <MOD-DIA><DIM>. You can add your own text and symbols to this area and it will be displayed in the dimension in the drawing. If you CTRL select more than one dimension the added text, number will be added to all that you selected. Make sure you do not delete the text in the <> as this will not allow the sizes to update with changes.
Hope this helps
Regards
Trevor
 

Ody_Mech_Engr

New member
Tony,

In the past I have just used manual references in the revision block to refer to the grid area. Our practice is to not modify locations of views or dimensions. Should a dimension be relocated and moved to a view or block, we would refer to it as "Delete Dim .153 from C7. Add Dim .155 to B6". Though trying to automate this is a very good idea just to be safe! Admittedly there have been occassions where I worked with a drawing that it was a judgement call whether it was C7 or C6. Generally though it was readily apparent.

Finally, if you find yourself repeating the same dimension over and over, you might want to consider referencing the number of occurences "7X .153" or "7X .153 MARKED 'A' " or "R .153 TYP" depending on the detail you need. Even if at a later date you need to break out one of the occurences and make it unique, it is a better practice to do so then, while using occurences now. Too much detail can clutter a drawing and make it difficult to read well. I've seen parts made wrong from overly detailed drawings as well as drawings lacking all the pertinent dimensions.
 

fcsuper

New member
Ovals

Once you are using Zones to establish where to look on a drawing for critical dims, you can then use another symbol in the DIM to ID which ones are critical quickly. If these are inspection points, you can use the ovals as well.
 

jamesdtuttle

New member
RE: Adding Numbers to Dimensions

Hi Tony
When you click on the dimension you will see in the "dimension text" box something like <MOD-DIA><DIM>. You can add your own text and symbols to this area and it will be displayed in the dimension in the drawing. If you CTRL select more than one dimension the added text, number will be added to all that you selected. Make sure you do not delete the text in the <> as this will not allow the sizes to update with changes.
Hope this helps
Regards
Trevor
Tony,

The method suggested by Trevor seems to be simple and straightforward. I'd recommend it over what I had in mind.

Adding identifying numbers to dimensions is not just good practice, it's an excellent idea. Using shops often do this for creating inspection reports, and the grid location data is something additional, rather than primary for this purpose.

Your users will bless you for saving them the work !

Best regards,

Jim
 

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