topic Linear Dimension on section view. in Inventor Engineer-To-Order (Read-Only)

Linear Dimension on section view.

Lesoux — Mon, 06 Jan 2014 18:33:58 GMT

Hi, everyone.

I want to add some dimensions (see picture) on section view. However, it seems impossible.

Sorry guys (Autodesk), but it MUST be.

Any ideas?

Re: Linear Dimension on section view.

Anonymous — Mon, 06 Jan 2014 21:24:21 GMT

Be more specific and we can help. What dimensions are you trying to add that are not working?

Re: Linear Dimension on section view.

Lesoux — Mon, 06 Jan 2014 22:05:12 GMT

Ok. Try to add any dimension from picture on the section view using ETO. Let's say groove inner face named "Face:1", groove outer face named "Face:2". Pipe outer face named "Face:3". The dimensions should be added on section view.

Re: Linear Dimension on section view.

Anonymous — Tue, 07 Jan 2014 22:39:45 GMT

Place workpoints in the model. Then use the workpoints as your entities in your dimensions.

Re: Linear Dimension on section view.

Lesoux — Wed, 08 Jan 2014 15:19:08 GMT

Not a good idea. So many additional objects. Need to be sure that you have section line in the right place. If the holes quantity will be changed? Need to control angle of section line location. All of it is performance. First of all my question was to Autodesk. This issue is one of the major problem in ETO drafting.

By the way, thanks everyone for response.

Re: Linear Dimension on section view.

JackGregory — Wed, 08 Jan 2014 15:59:00 GMT

First, some comment about this forum. When you post here, you are asking everyone for advice. That is why we support this medium. Often, the answers from users are better than we can give. After all, most developers have only a small range of the product they are familiar with. This case in particular, our resident expert is on holiday. I deliberately didn't answer because I didn't even understand the question (and am still not sure). I hoped someone else could answer. If you have a question for Autodesk, use the support channel of ADN. We will often direct you that way if it is not a general question that others can benefit from.

There are a great deal of difficulties with rule-based dimensions, and with them on Inventor. Seconday views, like sections, are even more problematic. The entities in the view often do not exist in the model, and the Inventor API isn't very good at letting us get to consistent mappings. So from the gate, this is going to be difficult to impossible. The advice on work points is good and sound. It is often the only way. You have all the rules, so you can figure out, with enough work, where they need to be. But it can be a lot of work, and may not be worth it. How to handle it is very problem-specific.

You don't say what you have tried to do, what the errors or results were, so it is really hard to help in any specific way.

Re: Linear Dimension on section view.

Lesoux — Wed, 08 Jan 2014 16:40:08 GMT

I didn't try give offense someone here. I just tried to figure out different opinions about my question (including Autodesk specialists) before creating some cases in ADN. About previous post with working point. I didn't say that it doesn't work. I just said that it's not a good idea. This is different things.

Thank you everyone for your responses.

Re: Linear Dimension on section view.

JackGregory — Thu, 09 Jan 2014 15:14:03 GMT

OK. The bottom line here is that because changes in rules/values can invalidate the view, it is re-created all the time. When that happens, anything in the view can disappear and be replaced with something else. The process of creating projections from Inventor models is not consistent, so curves (includes any projection of an edge) do not reliably appear. Any rules trying to get their endpoints, for example, will fail. So the advice to create work features and dimension off of them is actually the only way to get reliable results.

Re: Linear Dimension on section view.

Lesoux — Thu, 09 Jan 2014 15:43:39 GMT

Just proposition. You know that any cylinder surface on the drawing (section/projection view) will has 2 edges. For example, if your model has entity name like "Face1", maybe Intent can split name on "Face1:1" and "Face1:2" from left to right. What do you think? It should work with cylinder surfaces only.

Re: Linear Dimension on section view.

Lesoux — Mon, 13 Jan 2014 17:30:43 GMT

The ClosestPoint1 and ClosestPoint 2 helps to define edges (base on circular surface) location in section view to create linear dimension.
This post is closed.

Example:

Child dim As :IvLinearDimension

part1 = youPart

entity1 = "youFaceName"

closestPoint1 = Point(1,0,0) ' if edge is located on the right from origin

part2 = youPart

entity2 = "youFaceName"

closestPoint2 = Point(-1,0,0) ' if edge is located on the left from origin

....

End Child

Thank you everyone.