topic Getting Started with Model Based Dimensioning in Inventor Forum

Getting Started with Model Based Dimensioning

SEC_MECH — Thu, 02 Dec 2021 02:04:54 GMT

I am playing with Model Based Dimensioning for the first time and have some questions.

1) Why is the standard controlled by the Document Settings and not by the Style Manager?

In a DWG I can use the Style Manager to set the decimal character (point or comma) and default precision.

In IPT MBD I use the Document Settings to set a standard. I normally use ISO but this standard has a comma decimal character and no landing lines for diameter dimensions. To get these options I have to use the ASME (mm) standard.

2) How do I set the default precision?

The Document Settings Units tab allows me to set the default precision for linear and angular dimensions but this only applies to a Sketch and does not affect MBD. In MBD it always defaults to 0.00 precision and I have to manually right-click each dimension and set its precision.

3) What governs the plane that the dimension sits on when dimensioning between two faces?

e.g. Here I have dimensioned the width (120.00) twice. Both times it was defined by selecting opposing faces but the two dimensions are in different planes.

4) Why isn't moving a dimension consistent?

In a DWG I can grab either the value or dimension line and drag it to a new position.

In MBD I can only drag the value (of a linear dimension) to move it. If I try and drag the line then nothing happens.

But if the MBD dimension is a radius or diameter then the opposite is true - I can only move the dimension by grabbing its leader line.

5) How can you dimension size of a part with draft and fillets?

Real world plastic parts have a draft and filleted corners. Such parts are typically dimensioned to the imaginary intersection of faces (as if the fillets were not there). In a DWG it is possible to define line Intersections when dimensioning. How would this be done in MBD?

Re: Getting Started with Model Based Dimensioning

pcrawley — Thu, 02 Dec 2021 03:14:38 GMT

1 - MBD is controlled by the Styles Library - but it's an odd one. You need to edit the styles in a drawing (idw or dwg) to make it work.

Follow these steps to make the 3DA dimension style available in your document styles.
Do the same for anything everything which has a 3DA option. (I think its ID, Leaders, Surface Texture, Text, and Weld Symbols.)
Edit the dimension style the way you like it (decimal point, decimal places, etc) and make sure the text style you use is also a 3DA style.
Save the Styles to the Styles Library
Open your Part (and any other 3d model template where you might want to use 3DA)
Update the styles - and note that your new 3DA styles are the things being updated.
In each template: Tools > Document Settings > Standards, and select the ASME standard you edited above. This saves you from being prompted every time you go to place some 3DA in a model.

2 - Setting the default precision - you just did it in step 1.

3 - What governs the plane that the dimension sits on? The Space bar. Click to place the dimension - and while it is still active (i.e not placed) tap the space bar to toggle through available planes.

4 - Why isn't moving a dimension consistent? Very good question. I don't have an answer.

5 - How can you dimension the size of a part with draft and fillets?

Add your 3DA to workplanes and axes - then turn off the workplanes and axes.

Although real-world plastic parts have drafts and fillets, the point you are trying to dimension to is not "real" - it is an intersection point in space. So it's probably not something you would expect model-based dimensioning to do.

Re: Getting Started with Model Based Dimensioning

SEC_MECH — Thu, 02 Dec 2021 04:11:27 GMT

Thanks @pcrawley . Wow, the guys at Autodesk sure know how to overcomplicate things. I think that they need a product manager whose main focus is consistency, feature intuitiveness and ease of use.

It looks like a work in progress so I think that I will steer clear for now.

I am not sure why the ASME standard selected in the part correspond to the ANSI standard in the DWG. Sure, both are American standards but one is not the other.

I managed to change the decimal character but could not get the precision to change, no matter which default standard I changed. The Update in the part file did not appear to do anything.

Looks like the standard that I would most likely use (BSI) is not supported in this feature.

Sad to see disclaimers on features - "This style is intended for use in modeling environment only to format 3D annotation. Modify this style at your own risk as not all settings have been tested to determine effect to 3D annotation"

You missed my point to question 3. I was aware of the space bar to change the dimension plane orientation. I want to set the plane depth. The two dimensions that I mentioned have the same plane orientation but have different depths and I did not know what governed that or how to control it.

Thanks for your detailed post. Cheers 😀

Re: Getting Started with Model Based Dimensioning

swalton — Thu, 02 Dec 2021 14:06:20 GMT

I have noticed that if I promote a 2d sketch dimension to a 3D Annotation, the 3D Annotation adopts the style of the sketch dim. In my case, the default sketch dim is a 3 place decimal and the default 3DA is a 2 place decimal.

I don't see a way to get the intersection lines as part of a 3DA. I even tried to show the 3DA in a 2d Print. No luck.