How To Measure The Resulting "Altered' Dimension After Applying a Draft?

larry_hawes

I really don't know how many degrees I want to Draft but I can probably get a grip on that final dimension to check my part but am not sure of the best way to measure the resulting Draft dimension.

I have chosen a top feature surface on a simple rectangular extrusion/remove feature then selected the 2 sides and 'drafted' them 'x' degrees.  I then selected the remaining 'surface' of the now smaller draft area. Started a new sketch and 'Used' the previous resulting 'draft' lines and then measured those distances.

Is there another/better way to do so? Video should help. Not sure why YouTube is not playing nice but here's another shot at a video.

http://www.youtube.com/watch?v=9C-ZheQKj0c

https://cad.onshape.com/documents/2a10797e268c04fe7f37fd50/w/c65785afe6e50776efa3a0a2/e/1b285cad3276fe119388476c

larry_hawes

OK So that's how you post twice I'll see if I can delete 1 post.

larry_hawes

No Clue how to delete a post. Actually very little clue on how to navigate any parts of this forum after using hundreds of different forum software this fella has me continually stumped.

larry_hawes

Apologies, not sure why YouTube is not cooperating....

MBartlett21

@larry_hawes

You can select the lines or whatever you want to measure in the part studio.
A measurement will pop up in the bottom right corner. Sometimes there will be an arrow on it which will give you more measurements when you click on it.

larry_hawes

Thank you for the comment and it is helpful but I think my question was a bit mis-leading or at least incomplete. I re-posted a video that explains more of what I'm looking to do. Not sure if this possible to calculate within OnShape or if it is an external calc applied to Sketch/Drafts/etc.

http://www.youtube.com/watch?v=9C-ZheQKj0c

Jake_Rosenfeld

Hi @larry_hawes

This is a pretty simple trigonometry problem:

Imagine this triangle is you looking along the side wall that you're drafting inwards.

You know y, it's the extrude depth.
You know x, it's the amount of edge you want to "consume" with your draft.  In your specific case .01 a.k.a. (.5 - .48) / 2
You're looking for a.

tan(a) = x / y
a = atan(x / y)

You don't need to do this calculation yourself, you can actually just put "atan((.1 in)/(.8 in))" directly into the draft angle input.

You can also make this a little more by making a extrudeDepth variable and then using that in both the extrude depth field and the draft angle field, so that if you want to change the depth, you can change it in one place and your .48 across the bottom will still be the same.
https://cad.onshape.com/help/Content/variable.htm

Another completely different approach to this that doesn't require any equation setup on your part would be to just sketch the exact rectangle that you want to go up to, and then do a loft subtraction between the two rectangles.
https://cad.onshape.com/help/Content/loft.htm
https://www.onshape.com/videos/loft

larry_hawes

THANK YOU JAKE!!

You made my crazy question actually understandable. Unfortunately simple trigonometry problems have not been simple for many years and had no idea this could be done in OnShape as you illustrate. I will try this on the real part as soon as I get a chance.

Again thank you so much for the time and assistance.

larry_hawes

Tried your suggestion and might be missing something simple. I can see the draft being applied but cannot get OnShape to accept the formula in the Draft dialog box.

Thanks again for any assistance.

http://www.youtube.com/watch?v=mrtGBxa1hOE

konstantin_shiriazdanov

also you might use loft command with remoove option using two cross sections, it would allow you to directly obtain desired shape in this case

larry_hawes

Thank you Konstantin but in the production part I think a loft would break some of the geometry, or at least I would probably manage to break the geometry with a loft..

Jake_Rosenfeld

Hi @larry_hawes

Really sorry about this.  I should've tried it out before posting, and made some assumptions that weren't true.  First thing, you don't need the quotation marks, they were just my way of saying "put exactly this thing into the box".  But what I told you to put in wouldn't work, sorry to create confusion.  What you'll actually want to put is:

atan((.1in)/(.8in))
or even:
atan(.1/.8)
since the units cancel out anyway.

The first weird thing that's going on here was this:
atan(.1in/.8in)
is interpreted according to standard order of operations where "in" is actually considered a multiplication operation.  So this actually worked out to something like:
atan(.1 * in / .8 * in)
atan((.1 * in / .8) * in)
atan(.125 in^2)
which the system wasn't happy with (atan takes a unitless input).

The other weird this is that I told you to type:
atan(.1in/.8in) in
which is
atan(.125in^2) in,
which is just a total mess.........

I'll go edit my origin post, sorry for all the trouble.

Jake_Rosenfeld

P.S. the reason it looks like that draft is working is because these "invalid expression" errors are actually refusing to let you commit that expression into the field.  What you're seeing is a draft of whatever was in that box before you edited it (probably 3 degrees since that's the default).

larry_hawes

Thanks again Jake, I tried the new formula and found we had approx. 10 times the draft angle needed. I believe (.5-.48)/2=.01 not .1 and the formula should read atan(.01/.8) which gives a proper and accurate angle for the draft. Again thanks so much for the help. Much appreciated. 

Jake_Rosenfeld

Thanks @larry_hawes

Looks like I'm having a hard time today