I have started creating sheet metal parts in CREO 3.0, and he problem I am facing is that whenever I give annotations to the part using "Show Annotations" tool it gives me thickness of the sheet metal part as single arrow pointing towards the thickness and dimension written over it. I want to show this thickness as linear dimension just as you show normal thickness of a part. I just cant find a way to do it help me out please!
Note: I am only allowed to display dimension using "Show annotations" tool, I cant give dimension manually, by selecting the dimension tool.
Image is attached for clarification.
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The only way I can think of is to add a reference dimension to your sketch.
In this case, I used the thicken command under setup - feature tools and then added the dimension. It's reference, but in the drawing, you can remove the parenthesis.
There are certain "rules" that companies (or people) make about using only shown dimensions that do not work in the real world, especially in sheet metal.
An other way could be to start with a solid part. You can define thickness as a dimension in this case, then convert to sheetmetal. You could also constraint this dimension to be equal to thickness with a relation. I've already done this way in some specific cases.
From my point of view the best would be that PTC allows to show thickness as a regular dimension, with a config option.
I definitely agree that you should be able to show as a regular dimension!!
Please clarify; you are making drawings of sheetmetal parts, and your company policy does not allow you to add dimensions to a drawing?
What about "annotations" added to the model before drawing is started? One of these could be a (manually added) thickness dimension...
Depending on how you are making your sheetmetal parts, and what the documentation requirements are, it may not be easy to create drawings using "shown dimensions" only. For example, feature dimensions do not get mapped to the flat pattern locations (when you show them on the drawing of the flat pattern, they point to the "formed" location).
Yes I am making drawings of sheet metal parts and the company policy does not allow e to add dimensions in drawing. I hav to add them in the model and call up from 3D model to the drawings.
For now i am manually adding dimensions of thickness to the 3D model but it should not b done this way, I have to use "show annotations" feature to use dimensions frmom model. But I guess there isnt really anyway of showing thickness dimension the way I want to.
Yeah, I feel your pain. I think your company's policy needs to change. There are times to make exceptions to rules... Good luck!
BTW, instead of dimensions, what about a model note you show on the drawing? - it would say something like "Sheet metal thickness is &SMT_THICKNESS[.2] (mm)"
If someone made the rule about shown dimensions in drawings only and your company actively does sheet metal parts, then someone within your company knows how to show the thickness in your company's preferred method. The thickness showing as a note is not a new thing. Although I agree that the dimension should be able to be shown as a regular dimension, your problem is that your company (or you) have made a rule that can not followed due to the software that your company has chosen.
You have 2 options, change the rules or use an admittedly bad work-around.