Do These Prints Make Sense?

[RJSakowski]

How do these look?

I'm bound a little bit by the features fusion 360 currently has, through from what i have read they are adding more drawing features in the future.

Looks good Dan. I have not done any drawings with Fusion 360 yet so I don't know my way around the 2D stuff there but here is a horizontal ordinate example from SolidWorks.

 

[davidh]

did i miss the diameter of the two smaller holes somewhere ?

 

[John Hasler]

did i miss the diameter of the two smaller holes somewhere ?

Lower left, section B-B.

 

[Dan_S]

Looks good Dan. I have not done any drawings with Fusion 360 yet so I don't know my way around the 2D stuff there but here is a horizontal ordinate example from SolidWorks.View attachment 116892

it took me a little bit to get used to it, but now that i understand the difference between all the work spaces, I can knock stuff out pretty quickly.

 

[vtcnc]

Looks good Dan. I have not done any drawings with Fusion 360 yet so I don't know my way around the 2D stuff there but here is a horizontal ordinate example from SolidWorks.View attachment 116892

Drawings like this drive me nutty. I can measure your part and tell you where you put the features, but does it match your design intent? No reference to features, just imaginary points in space. What should the diameter or depth of the groove to be, for example? I would dimension the edge of the groove from a known end of the part and then dimension the width. Then I would dimension from the OD to the ID of the groove. Sorry to be critical....too many years of inspection experience!

Edit...the sheet2 drawing shows the depth of the groove properly. It's the attachment provided earlier (116892) that is not easy to interpret. Measuring a groove isn't easy especially if the feature is an angle. I have to say on this part, it doesn't look important...aesthetics only, so I would call out fractional dimensions here if possible. How will you do the 80 degree angle? Custom ground toolbit?
Sent from my Nexus 7 using Tapatalk

 

[Tony Wells]

80° easy. Plunge a CNMG with the correct nose radius. Or CNC, profile it with a UNR insert.

 

[Dan_S]

Tony has it, C shaped insert with the proper tip radius.

 

[uncle harry]

In section BB, you have over-defined the horizontal measurements. You should not have the overall dimension and the three dimensions adding up to that overall (1.250 and .250+.920+.080). as a machinist would not know which dimensions match your design intent. I would guess that the .920 dimension would be the one to leave off the print but that may be a critical dimension for you. From your block tolerance of +/- .003", if all the dimensions stacked unfavorably, the .920 dimension could be as small as .9111 or as large as .929.

That said, I often over-dimension on drawings for my own use because 1. it is convenient for me when I am in the shop not having to do the math to check a measurement and 2. because I know what the design intent is and which dimensions are critical. I have used parentheses around a dimension to indicate for reference only for drawings sent out to a job shop.



Another way to dimension horizontal and vertical positions is to establish a reference point and dimension using horizontal and vertical ordinates. The advantage of this is twofold. 1. There is no tolerance stack up as there would be when chain dimensioning. I use it when I have an array of features because a +/- .003" tolerance means that the feature is located within that tolerance at the nominal position. and 2. When actually machining, I will pick a reference point on my workpiece and all my machining positions are measured from that point.

For the hole positions, I would dimension each hole position from the center. Another way would be to draw a bolt circle and dimension the diameter. It wouldn't hurt to extend your center lines and add center lines for each of the holes. This will reinforce the location of the hole centers on the horizontal and vertical axes.

I usually do not put surface finish on a drawing unless it is critical. I have found that every machinist has a different idea of what a good part looks like and no two machinists will make the part the same. To that extent there is a component of artistry involved in machining. When sending work out, you quickly learn which machinsts do good work and which do not. Putting a surface finish on a drawing technically requires the machinist to verify the finish which adds extra cost. We did however, have some information in our title block

I generally don't use GD&T but it does come in handy when specifying things like perpendicularity, cylindricity, parallelness, etc. that would be hard to describe otherwise.

The important thing is to define your part in an unambiguous way. If you are machining the part yourself, it becomes very obvious if you have underdefined or overdefined. If you doing this in a work environment, you probably have a set of drafting standards to guide you.

Bob

An excellent description of good dimensioning practice. KUDOS +

 

[Wreck™Wreck]

I make parts from drawings every day, for the last 25+ years. A drawing made by someone that has had experience operating a machine is obvious as opposed to someone that has the skills and knowledge to design a part yet has no practical experience at actually making one.

Global Tolerances as used by many CAD systems (specifying a ± .002" in the attributes for example) will apply to all dimensions whether needed or not, this causes much consternation on shop floors daily. This often requires manually editing each unimportant dimension and removing the tolerance, if one were to draw the part with the unimportant features well smaller/larger the machinist would still be required to hold the stated dimensions and measure them. Also only put a surface finish callout on the surfaces that require it.

When preparing a drawing that will be used in the quoting process any unnecessary close tolerances or difficult to measure dimensions will add to the cost. Quite often the person making the part has no idea what it does.

 

[Wreck™Wreck]

Drawings like this drive me nutty. How will you do the 80 degree angle? Custom ground toolbit?
Sent from my Nexus 7 using Tapatalk

Program it, angles are easy in 2 axes however this would require doing the math to arrive at the points.
When I make lathe parts for my own use I draw them as pictured below, this gives absolute tool positions and makes programming easy, this approach also applies to manual lathe work but the angles are ground on the tool rather than interpolated or made with the compound of course.

This part would require 10 lines of position code at most on a 2 axis lathe.