Radius dimension not in the correct 2D view

Hello
I am rediscovering Solidworks after many years on Creo.
On the drawing, I want to show a ray from the model. Unfortunately this one is not in the right view and it is impossible to make it appear in an orthogonal view. It's particularly stupid and frustrating.

Do you have a solution to manually define a plan for laying the dimension?
The goal is obviously to retrieve this dimension on the drawing by object of the model.

On the 3D, by right-clicking on the offending dimension, it offers me "select the annotation view". I firmly believe that this is the option I need, but it doesn't work. The dimension does not arise on the plan I indicate to him.

Thank you for your help.
Onï

Hello

normally if you select your view and do Insert==> object of the model and you select your dimension parameters it should work.

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As you can see, he keeps telling me that the dimension is not parallel to the drawing views. :confused:

I sympathize... my return from Creo is not always rosy either.

If it helps you, a topic I had opened on more or less the same theme:
Dimension of a Plan as an Object of the Model - 2D Plan / Drawing - myCAD Forum (visiativ.com)

And I particularly recommend my last answer (a return from Visiativ following the opening of a ticket)

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What options did you choose to carry out your leave?


With these options I get the dimension via object of the model without any problem.

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The leave goes all the way

I reproduce the problem when I enlarge my radius and the radius cannot go around without interruption:
With problem


No problem

With the radius of 4, the coast changes to red (error)
image

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Thank you for this feedback,
I followed the last answer. it makes me see the dimension on a completely arbitrary view and I can't drag it on another view... Is that my problem!!
image

But, WHY IS HE SO EVIL??? :sob:

It's still surprising that he doesn't want to put himself in the right view once you've uncorrelated your rating from a specific plan.

Afterwards, I sometimes rate in a way unknown to Visiativ support (and there, we say thank you Creo). And it helped me out a few times.
That is to say that I select the function in my construction tree rather than on the plan.

To do this, go to the " template object" function, select your usual options. Put yourself in " selected function" and " destination view(s)"... in short, the usual little charms!
And there, hold on to your briefs for the manipulation: at the very top, you have two logos. One that looks like a stylized plan and another that looks like a nomenclature. When you hover your mouse over it, you'll see " FeatureManager Creation Tree" or " PropertyManager "
Select the first one (FeatureManager creation tree) You will then see on the right of your option window your tree appear: expand it. You have to choose the right leaf and then the right view before finding the construction tree of your model... It's up to you to select the function that works well now.

I'm not saying it's magic, but it has helped me out a couple of times

Edit: on the other hand, be careful: Solidworks displays all the dimensions and you have to delete them afterwards. Unlike Creo where you could select what you wanted to display (I've complained a lot of times after Creo, but I almost miss it now!)

Thank you for the trick, I knew the way to do it but that's not the root of my problem. What annoys him is that this radius dimension is not in a plane parallel to the views of the shot. So he doesn't want to ask it.
Hence my questioning, how to manually modify the installation plan of the annotations and dimensions.
Sadness :sob:

Edit: For the drawing, CREO is light years away from Solidworks.

As much as for me, I thought that you had already done the trick of linking your dimension to a plan and that it still didn't work.

So, you need to double click in the 3D on your function to make your dimensions appear. Right-click on the desired dimension and then choose

selected entity

and select either the plan you are interested in to link the dim to it, or choose " unaffected objects" to leave it free of constraints (which I recommend ;))

The thing where it's super intuitive is that you have to click on

Select Annotation View (*Face)

" to have the drop-down menu when you already have an impression of selection!

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Hello

I don't know if it's intentional but because of your geometry your radius is in 4 pieces.
With this option:


You will only have one surface and the dimension should be imported (if the geometry passes).

Nb: Particularly useful for surfaces made in ' simple ' machining. Solidworks has an annoying tendency not to keep the surface continuous (painful for us who machine a lot but practical for those who do foundry)

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I think we found the winner: @froussel

image
With this option it is indeed much better.

Thank you all for your involvement.
The solution found works BUT it changes the definition of my part and it no longer corresponds to my expectations.
I reworked the shape of my piece starting from a piece entirely revolutionary. So my R4 is not cut off and is on a plane parallel to a view. In addition, this new design will be easier to manufacture.

Have a nice day
Onï

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Hello

For your information this is a bug, currently listed under the number SPR 793227 - Can not change the chamfer or fillet callout at a hole edge to other annotation views. The topic is open on the publisher's side, and there is no particular workaround indicated. The solutions given above can therefore help.

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