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Sketching and extrude confusion
thomas_holford
Member Posts: 36 ✭✭
Reference document: Simpson Strongtie A35 framing angle
https://cad.onshape.com/documents/13e5e699cf0a40cf9565ee0c/w/cb1a6326c0da44a0a1919bb0/e/1c54bb347c0e46b8a13a8599
I am trying to construct an L-shaped connector with a bendable tab.
I imported a number of .dwg files and a text file and a .pdf file.
I opened A35.dwg in the Top plane of Part Studio 1
In step 1, I selected the thin edge of the flat drawing and extruded it in the z-direction.
I then tried various approaches to select the outline of the part on the Top plane and project ot 0.05 inches to create the other leg of the L-shape.
I cannot find a successful way to make this selection/projection work. OnShape will select the holes in the part and extrude them, but I cannot de-select the holes and select the outline. What I would really like to do is select and extrude the outline ans subtract the holes.
Also, there seems to be some sort of linkage between the Top plane part drawing and its mirror image, also on the top plane. When I select or deselect a hole in the drawing, it performs the same selection in the mirror image sketch.
Help. How can I select and extrude the part outline.
https://cad.onshape.com/documents/13e5e699cf0a40cf9565ee0c/w/cb1a6326c0da44a0a1919bb0/e/1c54bb347c0e46b8a13a8599
I am trying to construct an L-shaped connector with a bendable tab.
I imported a number of .dwg files and a text file and a .pdf file.
I opened A35.dwg in the Top plane of Part Studio 1
In step 1, I selected the thin edge of the flat drawing and extruded it in the z-direction.
I then tried various approaches to select the outline of the part on the Top plane and project ot 0.05 inches to create the other leg of the L-shape.
I cannot find a successful way to make this selection/projection work. OnShape will select the holes in the part and extrude them, but I cannot de-select the holes and select the outline. What I would really like to do is select and extrude the outline ans subtract the holes.
Also, there seems to be some sort of linkage between the Top plane part drawing and its mirror image, also on the top plane. When I select or deselect a hole in the drawing, it performs the same selection in the mirror image sketch.
Help. How can I select and extrude the part outline.
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Best Answers
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peter_hall
Member Posts: 196 ✭✭✭
This is why I created a solid with extrude command on the imported dwg file then used this geometry as a reference point for rest of the sketches to create the full item. To try to manipulate imported geometry that was not created on Onshape is giving oneself problems to deal with.5 -
matthew_menard
Member Posts: 96 ✭✭✭
Keep in mind that this is not a limitation of OnShape specifically. I never bother to use any of the *.dwg files the company I work for has. This is because the drafts-person before me drew everything at sheet scale, didn't use snaps to ensure line endpoints were coincident, and overrode dimensions all the time. In my case, it would be more work than it is worth to bring the existing 2d drawings we have into our 3d drafting program because I would just have to redraw everything anyhow. Peter's suggestion is probably the best one for 2d drawings that have never been used to create 3d geometry. This is because the 2d drawings can look great on paper but have flaws that make them unsuitable for deriving 3d solids. As you have discovered, some of the big flaws in 2d drawings can be: Endpoints not coincident, lines overlapping each other, small line segments that interfere with having a single closed loop, and geometry that isn't the correct size as what is called out on the print. Also, the imported 2d geometry is lacking constraints that will probably need to be added if you do any modification. By using the imported 2d drawing as a template that you reference to with your other sketches, you should be able to avoid most of the pitfalls mentioned.thomas_holford said:
A helpful answer. Maybe not the complete answer, but I'm getting the picture that imported dwg files are not necessarily always "ready to use".peter_hall said:This is why I created a solid with extrude command on the imported dwg file then used this geometry as a reference point for rest of the sketches to create the full item. To try to manipulate imported geometry that was not created on Onshape is giving oneself problems to deal with.
5
Answers
The original dwg has not been sufficiently carefully drawn, for instance if you zoom it at the junction of the two highlighted lines in the screen capture below, you will find a gap.
There are currently no diagnostic tools in Onshape for easily discovering such problems
My feeling is that we need a "select chain" function, as a start. Using this, having clicked on a starting entity, it will select all adjacent, properly trimmed entities. When it arrives at a gap, the selection process will halt.
The one in Solidworks functions well, but it works instantaneously. This presents a problem if you happen to pick a starting element with a gap at one end.
Solidworks' "select chain" will not reveal this problem, because it will run right round the boundary and select all the elements, arriving at the entity which lies on the other side of the break from the "far end", leaving all elements selected and the break camouflaged.
Better than slowing it down, I think, would be the ability to optionally to propagate the selection in one direction only, or the other, to more quickly discover breaks. Lacking that, it is sometimes necessary to iterate the process methodically, or make temporary diagnostic deletions.
If a few users upvote this post, I will raise an Improvement Request, called "Select Chain"
I would clean-up and be sure the sketch is fully defined before proceeding.
While I agree with you on the housekeeping merits of fully defined sketches, Onshape does not strictly require the endpoints to be connected, as long as they coincide (in other words, they do not need to be constrained)
When I dragged the endpoint of the highlighted line and snapped it to the arc endpoint, the OP's problem disappeared: the desired portion of the sketch became available for extrusion, without even needing to get rid of extraneous lines.
If it was me, at that point (provided I didn't wish to edit anything, and given that it's a commercial product, that seems unlikely) I would simply box select everything and choose "Fix", to safeguard against future accidental drags affecting sketch geometry
Thanks
Keep on Onshapin
When I box select a sketch and RMC I do not see a fix option. Please explain your last comment in more detail for me, it would be good learning!
Below image show option available in google chrome for changing window browser view
I'm so glad you were around to answer that question on my behalf with your usual thoroughness and clarity- I had forgotten about the browser window size issue.
Ideally there should be an "overflow indicator". I reckon, like in (mumble mumble) Microsoft Word toolbars, to alert people, particularly unfamiliar users, that they're not dealing from a full deck of cards.
Document: Simpson Strongtie A35 framing angle
https://cad.onshape.com/documents/13e5e699cf0a40cf9565ee0c/w/cb1a6326c0da44a0a1919bb0/e/2771d8d0c88645d581b01796
Tab: Parts Studio 2
Basic question: How to align Sketch 2 on Extrude 1 to Extrude/remove tabs and holes.
I imported a drawing to create the basic L-shape extrude "Extrude 1" The extrude surface is coincident with the Front Plane.
I imported a second drawing with the hole and tab locations, also on to the Front Plane. The hole and tab drawing is rotated 90 degrees from where it needs to be and offset.
I tried fixing the second drawing by deleting and recreating all the lines to ensure that all the vertices were coincident. I gave every line segment a relationship, like perpendicular, parallell etc. The drawing remains "unconstrained".
I tried relocating the drawing to the extrude by applying a coincident relationship to the top left corners, and then a parallel relationship to the corresponding top edge.
The result was that elements of the sketch moved but others didn't move.
I assume that answer is that the sketch has to be fully defined before the move, but then if it is fully defined, that would seem to make it immovable.
Help. How do I get my sketch aligned with the extruded part stock?
couldn't work it out tried a different approach.......any help to you?
I think I came to the conclusion that it wasn't workable for the following reasons:
1. A Parts Studio has a single origin.
2. An imported 2D drawing (*.dwg) may need a lot of fixing up to become "fully defined". There may even be things about imported drawings created in "alien" software environments that may be unfixable. In the drawing I imported, some of the points on the drawing appeared to be "fixed" without being flagged as fixed in OnShape sketch.
3. A drawing imported into a Parts Studio becomes a fully defined sketch when a point on the sketch is tied to the Parts Studio origin.
4. When a sketch is fully defined, it cannot be moved relative to the Parts Studio origin. Therefore, it can't really be manipulated relative to an extrude, and it really can't be positioned as a template on an extrude.
Possible alternative approaches:
1. It may not be possible to create a 3D part in a single Parts Studio using three orthogonal part drawings. However, it might be possible to import the three drawings into three geometrically corresponding planes, control the creation of the depth of the extrude along one axis of the extrude, and then perform extrude/remove operations from the other two planes to create the hole patterns.
2. Option 2, is to import each drawing into a separate parts studio, extrude the sides of the angle separately, and then combine the individual sides in a separate assemble tag, and merge them with the "combine" operation.
Ultimately, it's probably doable, just not easily doable.
"Use" can create a sketch from a part.
My premise that a sketch cannot be manipulated (translated, rotated, aligned) after it is fully defined seems to be true.
So, in order to import a sketch to use as a template for a hole pattern or something similar, it has to be imported to the intended location, orientation, scale, and alignment.
I guess the implied answer is, import the sketch, and then use transform to manipulate the part TO the sketch.
But then, at the end of the day, it is probably just simpler to make separate parts in different Parts Studios and assemble them using mates.
A sketch can be used as a template for a operations on a part by using the "Transform" operation to translate, rotate, and scale the part to coincide with the sketch. The sketch cannot be moved or realigned against the part.
Your following premise is incorrect: refer next reply
There is currently no easy way AFAIK to fix sketch entities relative to each other without also fixing them absolutely (to the origin).
The tools exist (in the form of constraints) to make this possible, but in sketches with significant numbers of entities, imported rather than created natively, it's so painstaking that it's not practical.
It would require a long essay to make this comprehensible to a new user, so I would suggest you work through the tutorial and video training if you want to get a conceptual handle on this.
One solution would be to provide a facility, with a single operation, to 'fully define' sketch geometry. This would permit adding the individualised constraints which leave sketches "mobile", and yet otherwise fully defined.
It works well in Solidworks, but an additional selectable category Onshape would require (because it behaves differently) would be "add coincident".
Alternatively to this last addition, I'm not actually sure there's any advantage in Onshape's different behaviour: can anyone suggest a benefit to the user from Onshape not providing an implicit "merge" constraint. as Solidworks does ? (not just for imported geometry, but for natively generated linework)
An alternative facility, which could provide a stopgap, and is also very useful in other contexts:
It would be excellent to have a "Group" capability inside Onshape sketches, preferably something simple (along Claris CAD lines), rather than the unwieldy "Block" in Solidworks.
The latter seemed tailored to provide something familiar for the Autocad user, and was not well thought out or integrated.
It seemed to me that "Derive sketch" in SW could instead have been enhanced with an optional "Name" facility, to facilitate multiple re-use. If Onshape did something along these lines, I reckon it could work in harmony with a simple "Group" command to render "Block" superfluous.
I'm thinking (and it's guesswork) that until you actually get some modelling under your belt, (not just sketching, but getting to the point where you can pick something off your desk and model it by several different methods) you won't have a conceptual framework on which to hang an understanding of sketch constraints which would be sufficient to prevent you making wrong or incomplete inferences, which can be a barrier to communication as well as understanding.
You have accidentally chosen an entry point (working from mediocre dxf/dwg imports) which is fraught with problems in Onshape at present. If that's all you ever will want from Onshape, it might actually pay to wait a while, until the capabilities catch up with what you're attempting. Values of "a while" are currently, AFAIK, unknowable.
I reckon that's great advice, to treat the imported linework as a sort of "reference underlay", and create a de novo working sketch from it.
It may prove helpful if the imported sketch is brought in at a different z depth (ie parallel to but offset) from the working sketch plane. This separation will let you view the two sketches simultaneously using pictorial viewpoints such as Iso.
It would pay to avoid snapping to the import's endpoints when creating the new linework: safer to "Use\Project" lines, then use the Onshape "Trim' tool, in case the Autocad drafter was not careful to produce properly trimmed geometry (no serious penalties for this particular lapse, within the 2D ecosystem)
The problem of dimensions being overridden during the lifetime of the original drawing is not revealed or alleviated by this precaution, but this defect is generally less common unless the drawings are from a rank amateur, because this particular flavour of 2D malpractice is likely to end up causing major ructions and rework in an industrial setting. Consequently the practice was likely to get someone fired if they didn't shape up pretty quick.