Foreshortened Radii and Linear Dimensions

[ptc-4245467]

I am running Creo Parametric 2.0 M030. How do I convert / make a shown model annotation on my drawing into a foreshortened dimension. I have two radii and a linear dimension that I would like to do this to. Using the Z-radius dimension is not an option (however the result of using this is the result I am looking for) and I am also not interested in some "workaround" that involves drawing a bunch of lines and other garbage on my drawing with a sketch. These dimensions need to be shown model annotations, no added dimensions are acceptable. See attached model and drawing. Sorry if I seem angry...Creo Parametric will do this to you.

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[James62]

Well, the following picture shows you the way how you should go on with this.

But it's buggered as you can see, and I have no idea how to get dim tol limits into model parameters. With dimension tolerance limit params you would be able to use those instead of the dimension parameter.

I guess with the bug there, your only option now is to write the stuff you want in the Z-rad dims manually behind the @O... The linear dim should work this way without a problem.

[TomD.inPDX]

Jakub is almost there. Yes, this is still a bug in M030 but you can get around it easily.

On the original dimension d6, remove the "prefix [R]" and add the R before the @D => R@D

Now you can create drafting Z-Radius dimension and overwrite the drafting value with R&d6@O

Someone really messed up the whole dimension formatting code somewhere along the Creo conversion. PTC development needs to go back to the original code and do a careful compare. Band-Aids are just not stopping the bleeding.

[TomD.inPDX]

The z-radius are re-associated to the original model dimension.

The linear dimension had the extension line erased which created the double arrow. After that, you can move the double arrow with the handle.

Files attached (Creo 2.0 M030)

[ptc-4245467]

Is there a way to put the "Z" zig zag like the Z-Radius dim into the linear dim?

[TomD.inPDX]

Although very appropriate on broken views, it has never been implemented as far as I know.

[ptc-4245467]

Isn't the double arrow in violation of ASME Y14.5-2009? I do not see that anywhere in the standard as a acceptable practice but the "Z" zig-zag is in the standard.

[TomD.inPDX]

You can blame the metric invasion

http://www.metrication.com/drafting/dim.htm

Many things metric are allowed in ASME 14.5-2009. They may not explicitely state such, however.

You might open a case with support to learn why PTC didn't adopt this age-old standard and what they have for the standard's association accepted alternative. The fact that we can do very little to arrow extensions in all of Pro|E/WF/Creo really makes this tough to live with. At least we can do what I have shown in the example.

[James62]

Nicely done, Tom.

@Justin: You can attach the linear dimension the newly created center of a Z-rad dimension.

[TomD.inPDX]

Glad you asked, Jakub.

Indeed, you can add drafting dimension to the Z-Radius dimension apex -and- it is accurate to the arc's origin.

Then you can replace the drafting dimension with &d13@O ... but you cannot use the underline font feature to denote the NTS status of the dimension.

Or you can format the drawing dimension, which is accurate, and use the underline text feature.

If you underline the model dimension, it does not transfer to the drafting dimension when used as above.

I don't really like either of those options if underlining NTS dimensions is a policy unless the dimension is not toleranced. Otherwise, you might change the model tolerance expecting it to change on the drawing.

Looks like another oversight by PTC developers.

[James62]

Ok. In my drawings I use rad dims that do not make this cross, or center of an arc, or apex as you call it.

So this arc center can be far outside the drawing. Since it's not displayed it doesn't matter then. I am guessing this can't be done to shown dimensions but only to driven rad dims created in drawing mode.

So that's another reason why not to bother with model dimensions in Creo.

What does NTS mean? Do you always have to underline the dim text if you make an incomplete dimension? I remember seeing underlined dims on a broken view somewhere, but I am not sure.

[TomD.inPDX]

Jakub, true that you do not get this option in model annotation. Silly but true.

NTS is "not to scale". This is the zigzag you see in some dimension lines where the true length is not represented. ISO introduced underlining the dimension value itself as an alternative. I have also seen adaptations where the dimension was appended with "NTS".

NTS is only used when both leaders are shown. In the case of the double arrow and erased leader on one end, it is accepted that somewhere on the drawing, you will find the appropriate reference for the "other end" of that dimension. I use it often when I have a view that has the dimension noting a diameter in a full section view (full dimension) and I have a detail view of only one edge with details. I will add the double arrow method to add a reference dimension to clearly note which surface is used as the reference or clarify a GD&T datum surface.

With broken view, again, you will see both ends of the dimension. This is where you most commonly find the zigzag in a dimension line. This is where ISO used the underline.

I wonder when the z-radius became more intelligent. I remember the post complaining about the poor control over the dimension's appearance. Today, there is a detail.dtl option as to what kind of mark you wanted at the false center, none, filled_dot or cross. default_z_radius_center_symbol

To add a linear dimension to the z-radius, you cannot specifically pick the false center, you just need to pick the z-radius dimension itself and it picks the false center as a point when you place the dimension. The linear dimension then recognizes the intended center as a reference for the dimension value.

[James62]

Ok, umm this question is kind of answered I would say, so I am going slightly off topic, but why I asked that one about incomplete dims.

Well, sometimes I do have a detailed drawing view where I would like to add dimension, not show since the model usually doesn't have any dimension, or not the one I wanna show. So there is simply only one reference for the let's say linear dimension, the other reference is cut out from the detailed view, obviously cause the detailed view shows only a detail or one side of a too tiny full view.

Would you think that it would be better if I created a completely new view, then put the dimension on it, that I want to shorten afterward, turn the view into partial, then scale that view up, so it's visible on the drawing, and of course erase the witness line of the said dimenson before I turn the view into broken one?

I am not sure if this is gonna work, but I would like to be able create these incomplete dims with double arrows on detailed-like views.

For the circle of a detailed view on the tiny full view I would make a dummy detailed view, and put that one outside the drawing border.

I am guessing this read is tough to follow.

Anyway, I guess we should call this done. Tom, you nailed it from up to down, and from left to right, and... I think that's good enough.

[TomD.inPDX]

I will play with that, Jakub. I will PM you with results. I think it worked much more reliably in Pro|E but Creo should be able to do this without too much bother.

Justin, I hope you are covered with more information than you ever wanted