Centerlines in Detail Views on Drawings???

[phlyx]

Have run across this quite a few times and wondering if someone has a 'trick' or way to get around this.  We often do dial indexing machines and the dial plate is a large round plate with multiple machined pockets around the dial.  We do a detail view of one of the pockets and dimension that.  The problem is the pocket is in reference to the centerline of the dial and that centerline doesn't show in the detail view.  And if we put a center point for the dial it's off the sheet and the centerline cuts thru other views.

 

Is there any way to put a partial centerline in a detail view without having to create a sketch and manually draw (fudge) a centerline in the view?  Cannot crop a detail view and also cannot break a detail view outside of the actual model.

[NigelHay]

Does Automated Centrelines in the detail view work? You might have to drag the centreline up so that it is close to your detail view & possibly position your detail view so that the centre of the centreline is off of the drawing sheet. You can still dimension to it but would have to select a foreshortened dimension line.

[phlyx]

Thanks but Automated Centerlines only adds centerlines to holes whose centerpoints are in the view.  Since the large diameter center is way outside the view, it does not add one for that.  Cannot dimension to a centerpoint that is off the drawing as it will draw a line from the centerpointto whatever you are dimensioning and you cannot crop or break the view.  Been fighting with this for a long time (years) and just got to the point to ask for hints.

[phlyx]

This is another example.  The arc on the part is much larger than the sheet.  Would be great if we could basically do a break on the view and have the centerpoint back on the sheet.  Then any dimensions that go to it would have the dimension line broken.

I just now found this post about the same situation from a couple years ago with some clunky fix to add a small bit of geometry where the center is so you can break the view.  Ugh.  Not a good answer at all and no real fixes.  Also, the link that @johnsonshiue posted to an Autodesk page doesn't exist  🙄

https://forums.autodesk.com/t5/inventor-forum/how-to-shorten-a-dimension-line-for-a-very-long-radius...
 

[phlyx]

Even that clunky solution doesn't work.  I put a Ø0.0001" extruded cylinder 0.001" long at the center of the radius.  Dimensioned it and then broke the view.  The linear dimension to the centerpoint showed up as broken, but the radius dimension still snaps back to the actual centerpoint.  And I cannot dimension the radius with a line to the centerpoint without it going to the actual center.

 

[mluterman]

Yeah, I'm getting away from centerlines (at the .dwg level) and starting to use features of the model as centerlines. For example, a projected midplane on a sketch in the .ipt for the sole purpose of having a centerline in the .dwg that is guaranteed to follow the geometry of the part. Then, in the .dwg, you do a "Get Model Sketches" and "Include" that same feature in the browser tree for it to show up.

[dhansenLXG2V]

So yes.  It can be done many different ways. I am going to assume that when you modeled the part that you referenced the "y axis" to pull a dimension off of when creating the feature just in the model?  Well the y-axis does still exist in the 2d dwg and you can use it just in the drawing view that you create.  First select the view and find it in the browser, click the plus sign and find the detail that you are working on, now find the base part (ipt), open up more and find all the base planes and axis', then you can RMB on that feature item and "include in dwg".  It is going to come in longer than needed, just grab a grip end and slide down to the length that you need. You can pull dimensions from and do what you need. The great thing about that is if a rev happens easy to work with. You can also do this with a created plane or axis'.  Hope this helps.?

[NigelHay]

The attached is what I had in mind. Automated centrelines creates a centre point outside of the drawing but you can dimension to it with a foreshortened dimension line. 

[CGBenner]

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@phlyx wrote:

Also, the link that @johnsonshiue posted to an Autodesk page doesn't exist  

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That post has been modified to remove the old link.  Thanks for pointing that out.

[phlyx]

Thanks @NigelHay, we can break horizontal and vertical dimensions but not a radius dimensions.  We need the line to the centerpoint or you don't know where the radius is being generated from and we need to define where that centerpoint is.

@dhansenLXG2V you said there are ways to do that.  With the last example I posted where there is a large radius and the centerpoint is off the sheet, please show a way (not manually fudged) to show the location of the centerpoint of the radius in relation to the model and also show that the radius is centered on that centerpoint with something like a line to center or placing the dimension inside the radius.  Really would like to know a way other than manual sketches and projected geometry.  

[phlyx]

@mluterman not sure how you pull a radius centerpoint dimension, even from the model, that is off the sheet and still dimensions the radius to it all in the drawing.  We still deal with shops that use the drawing to program their CNC's so they need dimensions on the drawing.

[NigelHay]

You can dimension to the centre with foreshortened dimensions & have a radius shown as a jogged dimension, see attached. The radius is added by including in the detail view, the sketch that defines the hole position. May not work for your programmers though.

[phlyx]

There is no validation that the R25.36 dimension is coming off the center of the circle in the main view and the radius it's dimensioning to isn't in the main view.  Any grey area on a drawing opens the door to get an incorrect part because of confusing or unclear dimensioning.  This is what I would like to be able to generate (which I can with everything except the radius). 

[dhansenLXG2V]

@phlyx  the center radius is quite a bit of a different animal and that is another question. You never replied to my first solution?

First comment, yes things can be done.  Will you have to "fudge" quite a little bit, yes.   Large machined parts and fine detailed dimensioning were always huge hurdles with Inventor.  I suggest that you learn more about model parameters and learning how is pull them into a drawing! IV does a really good job with part detailing and sometimes you have to fudge the visual representation but I always tried to get the true dimension or value from the model in case of a revision or change!!

[phlyx]

The example shown is the base structure of an actual part we're working on.  Attached is the part in my drawing examples, please show us how to dimension the large radius, defining the location of the centerpoint in reference to the part geometry while showing explicitly that the center of the radius is where the centerpoint is.   And this needs to be done so if any of the geometry changes the dimensions, lines and arrows all update automatically without any manually overriding.  We'd really like to know how to do that.  Thanks!

[SBix26]

It can't be done per ASME (US) standards, and I've been complaining about it for the last decade or more.  I think all of the Ideas forum posts have been archived, so the message is pretty clear that it's not going to happen.  Workarounds are all we've got.

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Sam B

Inventor Pro 2024.2 | Windows 11 Home 22H2

[dhansenLXG2V]

@phlyx I want to walk you through a couple things.  For a center point that you want to "show only" for reference there will be a few steps involved however if there is a change it will be easy to adjust so here is a quick walk through. I have attached views and the base part and dwg for you to reference.

It doesn't really matter how you created your view.  Select the view you want to work with, click sketch, you are now just sketching on that view and it will stay associated with it, especially if you move it or whatever. Create a centerpoint with lines (see Base004) that will be your reference CP and exit the sketch. Again you must select the "View" before you start the sketch. Click leader text and select the outer radii, pull back to visually get the leader to cross through the CP, enter "XXX" for text and close.

You need to setup a link from model to dwg. Go to model, open "parameters", add user parameter and name it, in the equation cell type the parameter name (see Base006), you must check "export parameter" box. Close and save.  Go back to dwg, edit the radii leader text, you have to select the custom parameter that you setup and click the import parameter button on the RH side (see Base007) and close. That dimension is always linked to the model, if the model changes so will the dwg.  I did a change to the radii to show you what would happen to the detail (see Base003). All that is needed is to re-adjust the leader to go through back through the center point.

If you want the dwg CP to hold a specific location you would have to dimension the CP in the sketch to reference base geometry.  Hope this help and at least gives you some ideas.