Help - I'm still doing math

Hi, I'm still learning some basics and have found I'm doing math more than I feel I should be, which makes me think I'm not being efficient at modelling.  I came up with a couple simple examples I'll post to see if I can get some advice on how to do it more efficiently.

Case 1: (Compound) miter cuts

Let's pretend this is something like a roof truss made out of 2x4 lumber (and lets pretend a 2x4 measures 2" x 4").  There's a horizontal beam, then a joist that meets it 30 deg below horizontal (just a single miter for now).  If I just make the 30 deg miter cut and butt joint the cut face to the beam, it's taller, as the vert. dimension of the cut surface is: L = 4" / cos 30 = 4.62".

So, if I want the cut surface to be flush with both top and bottom of the horizontal beam, I'd need to cut down the width of the 2x4 first.  So I could do math: 4*cos(30) = 3.46", draw a beam as 2" x 3.46" then cut the miter.

But I figured this is easier:  Draw 2x4 profile on front plane, draw a sweep path on the right plane 30 deg below horizontal, then do a swept boss/base, then finally square off the free end such that it isn't mitered.  This also gives me a width of 3.46".  This seems to work whether I select the Profile orientation to be "Follow Path" or "Keep Normal Constant", so I suppose I'll have to read in to the difference between these scenarios to understand better.

Now this is where I get stumped.  Now say this is a compound miter cut: 30 deg below horizontal, and 45 deg back.  Now say I still want the cut surface to be flush with top and bottom of the horizontal beam (so I'll need to wind up with the width of the beam to be 3.46") but I want to maintain the full 2" depth of the beam as it still fits fine.  E.g. I do not want the depth to become 2*cos(45)= 1.41"

So the only ways I can figure it out is I either do math manually to get the 3.46" dimension, draw a beam then make a new plane to perform the compound miter cut.

OR

I do math manually to figure out the projected depth 2/cos(45) = 2.83", then draw a profile 2.83" x 4", make a new plane to draw a sweep path on, then sweep along the path resulting in beam dimensions of 3.46" x 2".

Is there a way to be able to get this shape without having to do any math manually?

(I have another example I'll post in a separate post in this thread)

As a preemptive thank you, I really appreciate how willing people are to help beginners on this forum.  I do more asking than contributing, but hopefully that changes sooner rather than later as I get more proficient.

Thanks

SolidworksParts And Features
Answers 21
SA
SA 2017-08-29 Best Answer

Make your sketch on the right plane and extrude the 2.000"

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TD
TD 2017-08-29

Case 2: Dovetail board (Linear Pattern reference geometry)

Simple example of cutting dovetail joints, I've attached a file of the pin board, but similar situation arises with the tail board.

So I drew the Cut-Extrude1 to have the proportions I wanted on the dovetail, then I played around with LPattern to see how many instances of the cut I wanted to pattern to evenly distribute across the edge of the board.  After deciding on wanting to have 6 instances of the cut, I then wanted to center these on the edge of the board.  I could not figure out how to do this without manual math.  I thought I could use an "Equal" sketch relation to make the space from the edge of the board to the cut the same on both ends of the edge, however the repeated dovetail cuts don't exist in the sketch, only as extruded cuts under "LPattern1".  Yet I need the dimension from the edge of the board to the first dovetail cut to fully define the sketch of the seed.

Again, any suggestions on how to do this without manual math?

TD
TD 2017-08-29

I get how this is (shockingly) simple for the single miter cut - easier than making a sweep path, but how do I make this work on a compound miter? 

Is the easiest to draw the above sketch on a new plane that was 45 deg rotated from the right plane, extrude the 2.00", then use the right plane to cut the second miter at 45 deg?

KM
KM 2017-08-29

hei Tyler,

try this for an example

use the roll back bar to inspect the build

there is no math involved

see how you get on- kelef

TD
TD 2017-08-29

Hi, thanks for the file.  This is how I was able to do it for the single miter cut as well, but then I got stumped trying to do the compound miter cut.

SA
SA 2017-08-29

Equations would be one way.

My second suggestion is a little off the wall because I have not done this type of exercise in quite awhile. You could also use the segment tool to create a line with 4 equidistant points, add a couple lines equal to half the distance between points, then use a sketch driven pattern.  My construction sketch is shown below.

Of course you need to finish the sketch and extrude

Then use the center of the first left point as the center of your cut.

Finally use a sketch driven pattern to complete the task

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TD
TD 2017-08-29

Case 3: Linking part geometry to other parts from the assembly (dovetail shelf)

Last scenario I came up with.  If I was building the shelf in the attached file, and my design intent was that it has 4 compartments, and the interior dimensions of each compartment was 13.25" x 13.25", how could I make it automatically update the spacing of the interior dividers (Pin board > Cut-Extrude2) based on the width of the interior dividers (french dovetail part).  E.g. if I wanted to make the french dovetail parts only 0.75" thick instead of 1.5" thick, then the overall length and location of Cut-Extrude2 of the Pin board needs to adjust accordingly.  I was only able to brute force this by doing math manually.

Thanks again!

(thanks for the heads up, I've attached the part files for the assembly)

SA
SA 2017-08-29

Something else you need to learn about SW.  When you upload an assembly, you must upload all the components that make up the assembly.  My only option is to load your file in large design review.

For you last scenario, I might use an external design table to drive everything you want to do.  There may be better ways but again, I do not do this type of work very often (I mainly do rolls, frames, servo drives; nothing as complicated as you are attempting).

SA
SA 2017-08-29

Are you trying to make something like this?

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JM
JM 2017-08-29
<p>Tyler Dubetz wrote:</p><p>...have found I'm doing math more than I feel I should be<span style="font-family: inherit;">...</span></p><p>Thanks</p>

I am very experienced at math - I seldom use math in SolidWorks.

The geometry does the math for me.

Looking at your design - I would recommend investigating Sketch Blocks and especially multi-body solids modeling techniques.

Edit: I almost forgot - when doing the multi-body be sure to include realistic clearances between mating features.

Edit 2: ...and make use of symmetry about the origin. (you can offset an extrusion from the origin plane - most of my sketches are on origin planes)

Edit 3: ...when a bit of math is needed - keep in mind that you can use reference (driven) dimensions in equations as well as driving dimensions),

SF
SF 2017-08-29

For case 1, I would model that compound miter in the context of the assembly. Extrude it up to the surface of the mating boards and let the angles work themselves out.

TD
TD 2017-08-29

Yes, exactly (in my text I said 30 deg from horizontal just so they weren't the same angle for clarity, but this is exactly the concept I was trying to do)

DS
DS 2017-08-29

Why not just break things down...

Make the 2x4

Add the mitered cut(s)

Add the cut to the top/bottom of the 2x4 so it matches up to the other 2x4

Trying to eat a porterhouse in one mouthful often is more complicated and time-consuming than simply taking bites...

SA
SA 2017-08-29

This was made with a single 3D sketch.  Maybe a little overdone as Doug Seibel suggested but all I was trying to do was show options.  It all depends on the complexity of what you are trying to do.  Less features can mean less rebuild time and less RAM memory.  It can also mean only needing to edit one sketch/feature instead of two or more when making changes.  However once you insert the part into an assembly I do not know the significant of any of my points.

TD
TD 2017-08-29

Would you mind posting the file if you still have it available?  I'll take a closer look at it this evening.

Thanks

JS
JS 2017-08-29

Using SW - forget math - barely ever need it, and when you do you can do your math right in the dimension dialog box.  Focus on design and Design Intent - https://forum.solidworks.com/message/740952?q=Design%20Intn 

SA
SA 2017-08-29

As I told Tyler, in my opinion, it all depends on the complexity of what you are trying to do.  I have seen people use ten features for what should only have taken two.  The ability to only have to edit one or two sketches I find is much simpler when trying to modify a model you did not create then trying to sort through ten features to make a change.  Take the part shown below.  It can be done several ways besides the two I will mention.  Using the pancake method, it will take 3 sketches and 3 extrudes.  Using the revolve method will take one sketch and one extrude.  In my experience, depending on design intent, either one may be more difficult to edit.  So which is he porterhouse and which is the simple bites?

(and yes John S, I know I should have moved this to your Kitty Dump)

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DP
DP 2017-08-29
<p><a __default_attr="177380" __jive_macro_name="user" class="jive_macro jive_macro_user" data-orig-content="Solid Air" href="" data-community-id="1"></a> wrote:</p><p></p><p>As I told Tyler, in my opinion, it all depends on the complexity of what you are trying to do. I have seen people use ten features for what should only have taken two. The ability to only have to edit one or two sketches I find is much simpler when trying to modify a model you did not create then trying to sort through ten features to make a change. Take the part shown below. It can be done several ways besides the two I will mention. Using the pancake method, it will take 3 sketches and 3 extrudes. Using the revolve method will take one sketch and one extrude. In my experience, depending on design intent, either one may be more difficult to edit. So which is he porterhouse and which is the simple bites?</p><p style="padding: 0px; min-height: 8pt;"></p><p>(and yes John S, I know I should have moved this to your Kitty Dump)</p><p style="padding: 0px; min-height: 8pt;"></p><p></p>

Read this article:

UPDATED & CORRECTED – Why do I have to follow the Rules! #SOLIDWORKS | Michael Lord

Courtesy of ​

Specifically, this:

Edit: I am not saying that you are doing it wrong.  Please don't take it that way.   Just pointing out a reason to have more sketches sometimes (not all times though).

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DD
DD 2017-08-29
<p>Solid Air wrote:</p><p>(and yes John S, I know I should have moved this to your Kitty Dump)</p><p style="min-height: 8pt; padding: 0px;"></p>

No.  Your post is better suited to this thread.  The Kitty Dump is for when we not only get off subject, but when we get so far off subject there is no help being given to the post's subject.

DP
DP 2017-08-29
<p>J. Mather wrote:</p><p></p><blockquote class="jive-quote"><p><strong>Edit 3:</strong> ...when a bit of math is needed - keep in mind that you can use reference (driven) dimensions in equations as well as driving dimensions),</p></blockquote>

And measurements, too! 

BS
BS 2017-08-29

Some of your later examples are more complex, but for this first one (and anything with simple lumber), you should learn to use the weldment tool.  Your miters can be made by trimming the bodies and you don't have to create the profile every time.  Then, if you want to know any of the details for cutting any of the beams to fit, you can just pull them out in a drawing.

...and after further consideration, since you can use all of the usual SW tools on weldment bodies, you could do the more complex joints as well - maybe set up library features for these.