Drawing Detail Miter Angle Dimension

[cadman777]

Hi All,

I can't figure out how to make a dimension on a drawing view.

Maybe someone in here has done this and has an 'easy' or 'simple' way of doing it.

The shop needs to see an angle dimension on the detail of each part.

The angle is the chop saw miter angle.

They need to see it taken from 90 deg to the length.

Here is how I'm doing it now:

The problem I'm running into is doing this when both ends are mitered.

That's what I need help with, as in this detail:

Many Thanks!

UPDATE:
A possible solution is to RMB on the part in the model tree and pick 'Include Work Features', and then pick the WorkPlanes. Then use either the StartPlane or EndPlane (or both) for one of the angle dimension pics. But that option isn't available for FG parts. Do the newer versions of Inventor make these work features available for FG parts?

Google search returned this result on this subject.

Maybe by 20-f'ing-50 this function will be added to Inventor?!

[NigelHay]

Perhaps there's an easier way but I would make a sketch in the drawing view, create a vertical line, end sketch & place dimension. Then go back to the sketch & make your line "sketch only" so it disappears in the drawing view.

[cadman777]

Thanks for that suggestion.

I have been doing that on occasion for many years.

But that method is unacceptable on detail drawings b/c there are 10's (sometimes 100's) of details.

In a word: RSI.

I need a quick and simple solution.

[blandb]

Yea, this has been a struggle for years. Are these frame generator components? If so, could you include the Start and end planes into the view to use as a dim angle? These would be the ends of the members.

If not FG, then maybe prior to cutting the miter, use a work plane on the end face. Or, maybe do a plane after the miter to include into the view?

[cadman777]

Thanks for your thoughts!

Great idea, I thought of that too.

Unfortunately I can't find any way to access those work features like I can with non FG parts!!

[blandb]

I'm not sure how you are creating your drawings, but I usually place the parts as "detail item XX" and then place that part independently...But should be able to find it in the browser and include the features:

[cadman777]

Yeah, nice!

But unfortunately FG part details don't show anything like that when the view header is expanded.

Instead, there's NOTHING.

Non FG parts have that list.

What year did this become available in Inventor?

Either way, it's STILL a PITA for a command option that SHOULD BE available when placing Angle Dimensions.

[Frederick_Law]

FG part can add miter angle to partlist.

Not sure if that's the "correct" angle.

[cadman777]

Thanks for that info.

Yes, I know that from past research.

But it needs to be 'visual' for the shop guys.

Gotta make it 'dummy proof'.

[Frederick_Law]

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@cadman777 wrote:

Gotta make it 'dummy proof'.

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That's your mistake.

Never under estimate .....

[blandb]

I'm not sure what version you are running, but this is an FG component. Please see attached video?

[CCarreiras]

Hi Guys!

You an vote for this idea here:

Angle dimension with virtual line - Autodesk Community

[cadman777]

Ha!...Half the guys in the shop can hardly read a tape measure!

During summer when the shop temps get up into the 100's, there's little 'thinking' going on.

The simpler/easier the better, right?

[cadman777]

UPDATE:

I went into the Customization forum inquiring of a possible iLogic rule for this.

Here is what is going on so far.

Look at Message 2.

I'm posting that thread in here b/c it may save some work for people looking for this 'work-around'.

[info7JY2S]

I found the quick and dirty solution for this is to use a centerline. Create the centerline. Then drag the ends of this line to snap to each extending point of the part. After that you can use angle dimension on the centerline

I agree this function should be included...

[ldutkaTUZ58]

My experience had me speaking to the most experienced of shop guy(s). They may have a system that helps them get the item made and making their job easier. That way, any fab drawings are already set up for their usage and get things done quicker. Good Luck.

[SBix26]

Maybe I'm missing something-- as of Inventor 2021, you can choose to place a linear dimension with the option Rotated to align it with something else in the view:

After selecting Rotated, I am prompted to select linear geometry, and the result is this:

As shown here, when selecting the resulting dimension, the alignment geometry is highlighted along with the dimension itself.

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Sam B

Inventor Pro 2025.1.1 | Windows 11 Home 23H2

[cadman777]

Wow, nice!

Can you do that with an angle dimension like I show in my original post?

😫

[SBix26]

No, there is no alignment reference.  The quickest way I found is to create workplanes at the ends in the model and include those in the drawing view.  While FG parts usually have the Start and End planes in the right locations, FG trimming operations can leave the part ends offset from those planes, so it's safest to create planes specifically for this purpose.  But it still requires the Include function in the drawing, resize the resulting line, and then turn off visibility after creating the dimension.

I really think the idea @CCarreiras linked above in message 12 should be implemented, but its current status is 'Future Consideration', which is not encouraging.  There is a more recent Ideas entry, though, which is still 'Gathering Support': Drawing dimensions to Virtual / Perpendicular Lines - Autodesk Community.  Vote for this one, perhaps request that the two ideas be combined to show more support.

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Sam B

Inventor Pro 2025.2 | Windows 11 Home 23H2

[cadman777]

Thanks Sam, but I doubt it'll be implemented before I DIE.

I quit sucking-up to the developers over a decade ago, b/c I realized that they are driven by masters who are driven by greed not by interest in end users.

Until the corporate structure of America is extricated from society, and every person in every business is held accountable for their sneaky, hidden, evil schemes, nothing good will come from Autodesk, nor any other corporation.

These simple drafting functions should have been implemented within the first few years of the software's development.