I have to create a sketch in a drawing. Everything is fine until I used sketch tool - scale. My dimension is now completely incorrect. for example my hole dia 4mm becomes 12mm. What should I use to keep the dimension un changed? Thank you
Left click View. Choose scale options in feature manager.
Right click Sheet. Select Properties. Define sheet scale in Sheet Properties.
Do not use scale and draw your sketches as needed.
SolidWorks = (Always Draw 1:1)
I did. but when I placed the model on the drawing it is too small. I was told to enlarge the sketch.
Increase sheet or view scale and not sketch scale.
You need to adjust the view scale - not the sketch...
When I RMB I don't see View scale option. Please show me. Thank you
It works! Thank you. But I think I should not sketch on the drawing at all. I should use the geometry from the model and change my view scale like John and Deepak mentioned. Thank you all.
I review this post and noticed this portion on your post sample. Do you mind showing me how you create 3D swept to connect one cable location to another? Is this routing?
I have something similar to this last time and posted the question. I was told to isolate the assembly and created a 3d sketch to draw a cable sketch. It work but I spent a long time to make it perfectly fix to existing geometry. Is there a short cut or quick fix to accomplish this task? Thank you
Chika Co, Sorry for late reply as I was AFK for vacation.
What you see was merely an imported STEP file from manufacturer. I did not create this, but merely used an open component to make a fast drawing to explain with.
I make a 3D sketch, (for example) with a 1" line then a 2" line protruding perpendicular from both the start and end points. I make these lines construction, and dimension them for fully defined so far. Then I throw in a spline using each of the endpoints, allowing it to automatically solve the in-between parts. One key point, then I relate the spline as tangent to the 1" line at its end. If there is an obstruction to move around, I can either Add Spline Point and drag it around, or sketch in orthogonal dimensioned construction lines to define it to.
Then, to make your cable Sweep, I would not use a Profile Sketch, but rather define the sweep as a circular profile with a measured diameter.
I use this method for cables, wires, flex tube, and hoses. The Routing package does this also as an Auto-feature as applicable to either flex tube or wires/cables depending on your license version, but I feel it has results which are less manipulable. The only advantage I find from that package in this manner is the Auto-route through fasteners like a tube/hose clip, as covered in a Routing training class exercise. Same thing can be added to a manually crafted 3D Sketch also, with tangent relation added to a through-axis.
Put simply, I think you're already doing it the easy way. I have no extra trick to that.
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