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View Full Version : Things I wish I could do sketching in SolidWorks



Dennis Harbin
01-25-2017, 07:15 AM
After using TurboCAD almost daily for 21 years there are little things I wish SolidWorks could do as easy as TurboCAD to speed up the sketching process. I Like SolidWorks but I'm spoiled.

I'm hoping other people know how to do some of these things in SW so I can learn how to improve my modeling speed.

I'll work on a list and keep posting things as I encounter and/or remember them.

Layers - I use layers to deal with clutter so you can easily turn things off. I can create layers in a poor way by creating multiple sketches on the same plane and then turn them on or off but all the inactive layers will be grey and hard to sort out what you are looking at vs setting colors and line styles on layers.

When you are drawing a line there is this annoying thing of wanting to keep drawing lines chained together like a poly-line. If I just want a line I just want a line. I like the arc at the end of the line but at times would like to control the center point of the arc while drawing not just the current 2 choices. To do it you need to stop and select arc and draw an arc then go back to drawing a line.

I'm used to having all my drawing and snap icons available to turn on or off what I need on the fly. I may not want to snap to the center of a segment or I may want to snap to the center point of an arc.

The same thing with creating construction geometry. Once you start drawing a line you can't just click construction and switch to construction. You need to select it first or after you are done.

All these things mean extra clicks and time spent finding an icon. The trim icons are buried so it always takes at least 2 clicks. If you want to extend a line it's a pain to get to the icon and then it seems you have to get it all over again to extend another line plus you can't type in a value to extend it, you have to select the line and give it a dimension or edit it's value, but if it was created as a midpoint line you can't extend one end by entering a value.

At times it would be nice to turn off relationship creation while allowing snaps so you can create geometry which uses something as the reference for easy creation but isn't tied to it. Not every relationship should be permanent.

When creating parallel lines like for laying out an airfoil in TC I select parallel line, pick an existing line and move the cursor or type in an offset value (+ or -) and it's done. I keep on creating parallel lines until I select a different function. In SW you have to keep going back to offset and starting over. It does remember the last value you used.

In TC I can set a reference on an object (temporary or permanent), like a corner or center, grab that point and snap it to another object.

The difference is speed and ease of use. I still like the 3D capabilities of SW but it's taken me longer to model a wound wire ferrule than it did to build the tooling and make over 100 parts.

http://nc3397.blogspot.com/search/label/Wire%20Ferrules

This morning I finally got it to work and I'm delighted. Now on to finishing the wing rib.

cwilliamrose
01-25-2017, 08:19 AM
Layers -- These are not part of the sketch tools, they are only available in the drawing mode. There have been a few times when I wanted to change the color of a sketch entity but only a few in the 19 years I've been using SWx. SWx uses colors to show the status of sketch entities so I'm not sure how you could do anything with colors in a sketch that would not conflict with the SWx conventions. Turning entities on and off using layers is not something I ever wished for while sketching. I can easily change an entity to a construction line and that seems to be good enough for me.

When you are drawing a line there is this annoying thing of wanting to keep drawing lines chained together like a poly-line. If I just want a line I just want a line. -- It is technique sensitive. If you click then move the cursor and click again it will do as you describe. If you click and hold while moving the cursor then release where you want the other end of the line you will get a single line.

I like the arc at the end of the line but at times would like to control the center point of the arc while drawing not just the current 2 choices. To do it you need to stop and select arc and draw an arc then go back to drawing a line. -- I'm not exactly sure what you're getting at here. I use hot keys for lines and common arcs so I don't have to move the cursor to select something most of the time.

I'm used to having all my drawing and snap icons available to turn on or off what I need on the fly. I may not want to snap to the center of a segment or I may want to snap to the center point of an arc. -- Again, I'm not following you here. When I go to create a second line I can start it on an existing end point, a center point, the mid point of an existing line or just some random spot along an existing line. The existing line will display a little icon telling you what you're about to select as your line's end point. I never sketch with the grid on so there's no snapping to the grid in my world.

The same thing with creating construction geometry. Once you start drawing a line you can't just click construction and switch to construction. You need to select it first or after you are done. -- You are correct here. I don't know why I'd want to do it on the fly....

All these things mean extra clicks and time spent finding an icon. The trim icons are buried so it always takes at least 2 clicks. For common commands I use hot keys or hot buttons on my Space Explorer. I hate using icons or even moving the cursor away from the drawing area.

If you want to extend a line it's a pain to get to the icon and then it seems you have to get it all over again to extend another line plus you can't type in a value to extend it, you have to select the line and give it a dimension or edit it's value -- You can drag the end point but that's not going the maintain the line's direction. I have hotkeys for trim and extend (T & E).

If it was created as a midpoint line you can't extend one end by entering a value. There is no extend tool that allows a value to be entered that I know of. I too find it a bit of a pain to extend a line that is currently terminated to another entity because I often create a quick temporary line to extend to, then delete that line so I can edit the length some other way. With hot keys I can do it quickly so it's only a minor bother.

At times it would be nice to turn off relationship creation while allowing snaps so you can create geometry which uses something as the reference for easy creation but isn't tied to it. Not every relationship should be permanent. I'm not sure if that's possible in all cases but you can assign a hot key to the Automatic Relations setting which will toggle it on and off.

When creating parallel lines like for laying out an airfoil in TC I select parallel line, pick an existing line and move the cursor or type in an offset value (+ or -) and it's done. I keep on creating parallel lines until I select a different function. In SW you have to keep going back to offset and starting over. It does remember the last value you used. True, I know of no work around other than defining a hotkey for the offset command.

In TC I can set a reference on an object (temporary or permanent), like a corner or center, grab that point and snap it to another object. Not sure I get this one. You can drag sketch entities or points around in a sketch but I don't think that's what you're looking for.

The difference is speed and ease of use. I still like the 3D capabilities of SW but it's taken me longer to model a wound wire ferrule than it did to build the tooling and make over 100 parts. -- I had a lot of these same issues when I came from CadKey. Now I don't even remember how I used to do things in CK anymore.

http://nc3397.blogspot.com/search/label/Wire%20Ferrules

You can make a simple part using 'Twist along a Path' in the Extrude-Sweep function pretty quickly. Defining a helix and then using that as your path is much slower. Doing an oval,,, I'd have to think about that one...

Dennis Harbin
01-26-2017, 06:26 AM
This is great. Thanks for the help!

I'll go work on the hot keys which I use a lot in both TurboCAD, CoreDraw, and my embroidery digitizing software. I'll see if I can explain some of these wishes better. I'll make better notes as I'm working. I like the colors and line styles of layers because they help me quickly recognize what I'm looking at. This is my wish list, but I'm delighted to learn alternate methods. I tried about 4 methods of creating an oval helix. They each had their issues, even if you make the sides flat which they are not in the actual parts. You can do a single turn with a spline or with 4 segments of helix's. The helix takes some thinking and math but it will work. Once a turn is created you need to create offset copies then join all this into a single object line with the connecting points tangent. Apparently the offset has math issues because I could join a few turns but I always got errors when trying to join all ten turns. Then there were issues cutting the angle on the extended ends of the wire. Apparently the plane you use for the object, to do the cut, needs to be parallel to the centerline of the coil at the end of the turn or again it has math issues and creates weird results.

OK I should have started with easier parts like my exhaust manifolds.

http://curtiss-ox-5.blogspot.com/

My first part was a bracket for the wing drag wires. It has a copper grommet where the wire goes through the bent tab.

I think the help needed is both things like tips on things like hot keys, but also ideas on what modeling strategies work. I made the cap strips on my wing rib using the sweep function, quick simple and it worked. Well, it worked until I tried trimming the overlapping ends and kept getting gaps, more math issues. I'm going to model them like I did the straight sticks by creating the outline in the front plane and the extruding them to 3/8" deep, goodbye gaps.

Can SolidWorks deal with nails? I know I don't need them but I'm learning and it's fun to do things just to see what works and how you can use different functions.

cwilliamrose
01-26-2017, 08:51 AM
I did my main capstrips as you describe and maybe for the same reason -- I seem to remember some problem with trimming. All the straight capstrips are a single file with different configurations for the various lengths. I referenced the Pitts part numbers from the plans for the configuration names. The gussets are two part files, one for rectangular gussets and the other for triangular gussets. They could have all been in one file but I did it this way for no real good reason that I can recall. Again, the configuration names come from the part numbers in the plans.

6072

By "deal with nails" do you mean within an assembly? If that's the question then yes SWx will do fine with them with one minor problem. If you 'drive' them flush or nearly flush with the surface the underlying part's appearance will tend to print through the nail head and be visible. The only way to avoid this would be to counterbore for the nail head. Since nails aren't really necessary in an assembly I assume the reason to include them is to make a rendering and that's where the C-bore would be important. If it's just to show them in a 2D drawing the C-bore would not be necessary. I'd make a sketch-driven pattern to place them in the assembly where you want them.

Dennis Harbin
01-27-2017, 06:05 AM
I've also made separate files for each of the parts in the rib. I've used the WACO part numbers for all the parts. Most of the parts in the WACO NINE wing are the same parts used in the model TEN. I'll have to create numbers for unique model NINE parts since only a few ever got part numbers. I re-did the cap strips and have my first gusset ready to assemble to the sticks. I probably won't put nails on. I found a cheap $5 nailer which saved 1 hour per rib nailing gussets. They showed them on the factory drawing and that prompted the question.

6084

cwilliamrose
01-27-2017, 08:58 AM
My rib parts are not separate files in every case, they are often one file with numerous 'Configurations' used in the assembly. Maybe TurboCAD has similar functionality?

The boxes in the image enclose some of the individual files used multiple times in the assembly. The parts in the assembly coming from these individual files are not the same, they are configurations of the same file. Each configuration describes a different version of the part. The part number for the cap strips starts with 1-437 (which is also the drawing number where they appear in the plans). The -xx is the rest of the part number which differentiates the individual parts on the sheet. The configuration's name appears in the feature tree right after the filename (blue arrows) and I used only the -xx of part number for the capstrips. The gussets use the entire part number for the configuration's name. I'm nothing if not inconsistent. :)

The Component Properties dialog is where you select which configuration will apply for each instance of the part. And notice at the bottom you can specify which configuration(s) of the assembly to use the various part configurations. Yes, both parts and assemblies can have configurations. Very handy for things like rib assemblies which can be slightly different versions of the same assembly with a few parts being swapped out for other parts to create a rib for a special purpose.

In the case of the capstrips 1-437-2 is different than a 1-437-7 only in terms of their lengths. But 1-437-41 is not only a unique length but is a different section -- ¼"x¼" versus 5/8"x1/4" which is used only in compression ribs. The configurations of these different part numbers have different dimensions assigned to otherwise identical geometry. In a lot of cases this is much easier than making separate files for each part. Being the lazy sort, I use configurations a lot.

6085

My rectangular gusset part file is used nine times in this rib assembly. Four are -2, the -7 is used twice and the -10_U, -11 & -14 are used once each. These are attached to one side of the rib, the gussets on the other side are mirrored. And yes, once you mirror or otherwise pattern components you can change the patterned version's configuration without affecting the parent's configuration.

Dennis Harbin
01-30-2017, 06:40 AM
I like your idea of using configurations. It will be really good for all my drag wires. I have some versions of this rib which might be easier to create that way also. Creating the straight sticks as separate parts from within the assembly was pretty quick, probably the easiest thing I've tried. They are all rectangular so it was easy to use a 2 point rectangle for the vertical sticks and a 3 point rectangle for the diagonals. For the diagonals I snapped the first corner a cap strip, the second to a vertical stick and the third point to the opposite cap strip. I then set the stick width to 1/4" and adjusted the length to the nearest 1/32" which would fit without being too long. I love the way the stick just moves into position as you adjust the length. The extrude function remembers the last value you used so it was easy to extrude the sticks to 3/8" deep.

The gussets were easy enough to insert in the assembly and then position with mates, as I did in my rib jig. If I were doing this again I would set my work plane to be in the middle of the rib sticks so it would be easy to mirror the gussets from the first side to the second side. There probably is some way to do the mirror with an offset and I just couldn't figure it out.

One problem I did have was trimming the gussets. WACO glued them on with a corner or 2 sticking out slightly past the capstrip, as needed because of the curve and then trimming them on a belt sander. I have a factory picture with a guy standing at the sander with a rib. I used a Formica router bit to do it with the router table, much quicker.

6098

When I tried using the Assembly Sweep Cut Feature I could not create a 3d plane perpendicular to the original sketch construction spline I created for the curve of the capstrip. I tried copying the curve to a new sketch but could not figure out how to position it in the exact position as the original curve. I wish I had the handle and snap functions from TurboCAD. In the end I just redrew it in a new sketch and that worked fine for both capstrips. I created a shape which trimmed the gussets with the 15 degree angle of my router cutter, very cool. However this apparently destroyed several mates. In the end I just deleted the damaged mates since the gussets are now in the position I want. I don't think the mates add any longer term value. The rib came out just like the real ones.

6102

I'll work on using configurations to make the other versions of this rib. Now that I have the wire ferrule I'll use configurations to assemble my drag wires, they should be easy.

Does anyone have models of AN turnbuckles, etc.?

I really appreciate your help and ideas.

cwilliamrose
01-30-2017, 09:52 AM
The router trimming works great in real life but you have to keep glue off the surface of the capstrip so the bearing is riding on a true surface. We just trim them off flush with the capstrip and use a sanding block to break the edges. I never thought to model a router operation with an angled cutter since I never thought to use one for this purpose. I wonder if you could just use a chamfer after doing the overall trim? Of course there's no fun in that.....

6104
Untrimmed.

6105
Trimmed and chamfered.

The one PITA with the chamfer tool is there are always a few edges that insist on having a backwards angle. Happened here too for my little experiment -- one gusset didn't cooperate.

You can use any plane or even a planar face to mirror components. Just create one for the purpose or use one that's in the part file for the straight capstrips. If you used a mid-plane extrusion there will be a centered plane in the part file.

As for leaving the gussets without full constraints, all I can say is they may move on you. I mated mine using features that would be trimmed off later but it did not disturb the mates since the trim happens after the mate in the feature tree.

I don't have any turnbuckle models, I don't use them in Pitts airplanes and that's all I have ever modeled in SWx. There are no pulleys in a Pitts either so I don't have those models handy. Maybe someone has posted turnbuckle part models on GrabCAD?

Dennis Harbin
01-31-2017, 06:30 AM
You're right about the routing of gussets. If there is glue or a nail sticking out the roller follows it perfectly.

I checked to see if the trim was being done after the mates and it is at the bottom of the tree. The mates are a couple lines higher. I wonder if I had left a .001" gap above the capstrip if the mates would have been preserved. I had this problem with the ferrule when I tried using the sweep to form the wire along the centerline. I accidentally used .100"dia. (the default) instead of .125" and it worked fine. when I changed the diameter it blew up. I made it .0005" smaller and it worked. There may be slight math problems causing the trim to wipeout some of the mates where the corner of the gusset is mated to the edge of the capstrip. I had to redraw the line for the edge in order to place the plane for the trim profile so they may be slightly different despite using the same points to create the lines. I need to figure out how to copy an entity and precisely place it in another sketch, or why it wouldn't let me use the original spline.

I see what you are saying about creating a plane 3/16" off the workplane to mirror the gusset. Lots of fun things to play with. I have a wish list issue form sketching the front gusset. I'll figure out how to show it and then get it posted. I think the neat thing is there are so many ways to approach any item, the trick is what works best for each of us in any situation.

Thanks,

cwilliamrose
01-31-2017, 08:05 AM
I checked my rib model to see if the vertex I mated to was still there -- it's not. And the mate is still satisfied. So this could be one of those SWx things where a chamfer acts differently than a swept cut. One thing I'll mention for future solutions to odd problems is that you can mate to sketch entities which can be handy sometimes. You can even go back and add a point or a reference line to a sketch if there's nothing in the right spot in the original sketches. Or you can add a sketch just to serve as a reference for mates. This can have practical benefits later on -- if you modify a sketch the resulting extrusion will often create new solid features with different ID's than the old ones which will kill any mates that used the old feature's ID. This is also true if you cut away part of a face -- what's left might end up with a different ID number than the full face had.

I always try to impress on new users that it is best to use the oldest feature you can find for mates or for converting edges to sketch entities. It pays off later when you edit the model and some of the more recent features change. By oldest feature I mean going as far up the feature tree as possible. Sketches are just slightly older than the features they drive and they aren't subject to be cut off the model like a solid feature might be....

Dennis Harbin
02-02-2017, 07:05 AM
I think what I'll do is make the next (shortened) rib from scratch to try some of these things rather than modify this file and carry along any junk I've created. Now that I know more about what I'm trying to do it should be much easier. I already have all the parts and I can redraw the sketch easy enough. I have one rib which adds a part to the side of this rib and I can do it as a configuration of the existing rib. That way I can try out more ways of doing things.

Thanks,

cwilliamrose
02-03-2017, 01:53 PM
Let us know how the next one goes for you.