How can I do manufacturing drawings when the way the model is built does not represent its manufac.?

[AB_10071442]

I have seen this video https://www.youtube.com/watch?v=Hky98wUL-jo&list=PLRhPac0z_f-FIsmKbE1fR1ZlEMXBZcZvN from David Martin on worst drawing practices. There, he says that most dimensions should come from the model. In this video https://www.youtube.com/watch?v=cxKmlE8afhs on worst modeling strategies, he says that you should not create your model in a way that represents manufacturing. But, when I make a drawing, it is mostly for manufacturing. And if I did not build my model in respect to manufacturing, then I can not take the dimensions etc. over from the model. I also have made the experience that when I make a new model, it is built up in a way that is different to how it is manufactured. For example, the lathe operator maybe needs diameters and everything dimensioned to one edge of the part. But, when I modeled the part in Creo, I maybe dimensioned a revolve in reference to another revolve. So they do not reference the same edge. Does somebody maybe know how to deal with this? Thanks for any ideas and replies! Please write if you need additional information or an example as a model etc.

[tbraxton · Accepted solution]

Take as an example a part machined from billet. You should probably not start your Creo model with a block of material and start cutting away at it (i.e. hack and whack modeling). This does not preclude you from building the geometry of the part using features and dimensions that reflect design intent as well as inspection dimensions. Keep in mind that you can add dimensions to sketches that are "extra" above what is required to regenerate in sketcher. Annotation elements also support the creation of dimensions (inspection) on the model to capture those that are not defined within a sketch or feature that you need for documentation purposes.

I have never encountered a situation where I am unable to add a dimension to a model that was needed on a drawing. If you post specific examples, I am sure you will get some recommendations on how to handle it.

About Using Annotations (ptc.com)

[AB_10071442]

Okay, thank you for your answer! So for example, I have a turned part which is made like in the video

Now, I want to ask the lathe operator to turn the part. So everything should be measured from the right surface. So I would go like in the next video

[tbraxton]

Example of dimeter dimensions in a sketch for a revolved feature.

This can be realized by the following:

Pick the axis, pick the radial point, pick the axis again, and place the dimension. (It can also be done, point, axis, point)

[BenLoosli]

You can create drawing only dimensions that will give the shop floor what they need. You do not have to use the Show Annotations function to dimension a drawing.

When it comes to modeling a part, I have always tried to model it as it would be manufactured. This will drive the dimensions in a more useful way for the drawings going to the shop.

[StephenW]

I am just going to say you will get so much variation on this topic based on opinion and experience. It's all valid. But not everything that is said will be right for you and your company. Take what you learn here, try it, modify it, make it work for you and your company. 

My guidelines are:

1. Design intent. - Dimensions, and references that make sense to what I am trying to accomplish.

2. Manfacturing - its important that your deliverable to the shop floor or vendor makes sense to someone who is going to build it.

3. Extra - because a list of 2 items is silly so i added a #3 to make me look smarter. No one reads this far down anyway.

4. Over and Above - now a list a 4 items because i'm just showing off how smart I am!

[BG_9869104]

To directly answer "how I get a model to display the dimensions on the drawing that are desired" : I open the model and redefine the dimension layout. Sometimes its a small edit sketch, delete one dim and move it. Sometimes I have to delete the whole feature tree(or start over with a start part) and start over to recreate the part properly. If recreating model I save the original as a copy and have it to compare and measure on. Depends on how jank the models you get fed are, how big they are, and how much time you have.

Types of drawings I have crossed paths with.

1. Design - Datums and dimensions based on design intent. Weighting of this depends on if the dimension layout makes a real difference. If you are fighting for microns in a stackup of tolerances and laying the dimensions out in a specific way for the shortest possible DVA loop then it is pretty important. Usually this will lead to a drawing that the other areas will not like unless they understand the WHY. 
2. Manufacturing - Datums and dimensions based on how the part will be held and made during manufacturing. My work just fine for design.
3. Inspection - Datums and dimensions based on how the part will be held and measured during inspection. Sometimes differs from manufacturing and design.
4. Assembly - Often found that assembly teams like to have directed access to a dimension and tolerance that may be a calculation with the existing drawing.
5. What someone in a position power decides
6. What can be slapped together in a short amount of time

Most of what I make are drawings for inspection with a heavy weight on design intent. Manufacturing and assembly specific items get the scraps of being added last if at all into model sketches and shown on the drawing. Where I have worked the addition of reference info is very limited and if not absolutely needed is not allowed on a production release. The more clutter that gets added to every drawing is the more clutter that has to be maintained over decades. Read, extra info cost money, big money if an error happens due to reference info on a drawing.   

[StephenW]

99% of my drawings!

The other 1%..."i'll just send the model and we'll worry about the drawing later!"