I have created a flat part, let's say it is a piece of steel plate. One edge of this plate has been defined with a spline because it is not a plain geometric shape. I have then created a sketch on the surface of the plate. In that sketch I have create a shape that I want to Cut Extrude through the plate. So far, one cut-out, no problem. Next I want to pattern that cut-out, following the splined edge.
First off, is it possible to pattern anything along a spline? If the answer is yes, what's the best way to approach this? I have been trying to create the pattern in the sketch, then Cut Extrude the entire sketched pattern in one shot. I'm really struggling with this and I cannot get it to work.
Should I be trying to Cut Extrude one of these features first and then later pattern that cut-out feature? I've been trying that too, but SW won't let me select the spline as the path to follow for the pattern. If I could select the spline for my path, I would like to follow or maintain the alignment of the seed.
SolidworksSketching
1. Create the Sketch with the Spline
2. Create one Cut as a feature (different sketch)
3. Use a Curve Driven Pattern
http://help.solidworks.com/2012/English/solidworks/sldworks/HIDD_PATTERN_BY_CURVE.htm
I'm having a similar problem that I can't seem to solve. The issue is that I want to pattern a bunch of holes along a curve where I want the X displacement to be equal (in this case 11mm) but the Y displacement to be along the curve. I started to do it by hand by creating coincident and tangent relationships but there has to be an easier way. I've tried the different curve methods and it doesn't seem to change anything.
If you look at the attached screenshot, the grey circles are how I want them - centered on the construction curve and tangent to the vertical lines. The yellow is what I get when trying to use the along curve pattern.
Any thoughts?
In your case you might need to use a sketch driven pattern. Place points at the intersection between the vertical lines and the curve and use the resulted sketch for driving the pattern.
I'm not sure that will get me what I want though. I want the holes to be centered on the guide curve and tangent to the vertical lines. Placing points at the intersection will center the holes on the vertical lines which is not quite what I'm after. I could offset the vertical lines by the radius of the hole which would be closer to what I want but still not perfect.
My bad, you are correct.
Have you tried the solid body way?
just like a drill bit you can use them and subtract using the combine tool.
it maybe easier because you can place the bodies with the move
copy body feature and mate them into position.
I'm not familiar with the move copy body feature (I'm kind of new to SW). Is this an automated process? I ask because I've got about 50 of these holes to do. Being the lazy type, I'd rather spend an hour learning how to automate the process rather than spend an hour doing it by hand!
Andy,
Why do you say that offsetting the vertical lines by the radius of the holes would be closer but still not perfect? It seems quite exact to me.
I think that is close as you can get to a reasonably fast process.If you are careful when you place the sketch points you will get the proper intesection relationship. (Watch for the intersection icon as you hover over the intersection.)
Jerry Steiger
A table driven pattern might work here. As long as you know the curve equation and are Excel savvy...
Yea, you might be right. The holes are 3/16 or .1875. If I offset the verticals by half that in the X and use the intersection to create the point, the feature would be tangent at the Y level! At least I think it would be. I'll try.
yep just did it, things we were taught in geom class.
Andy,
When Alin replyed to my original question he gave a good answer on how to achieve what I wanted. What he didn't say was the SW will NOT allow you to create a pattern on a spline in an active sketch. I arrived at this conclusion by reading between the lines on Alin's response and by reading other threads.
Instead, you can create the spline in a sketch using the normal tools for doing that. Then create your seed shape for the pattern and close the sketch. Then cut-extrude the shape into your part. Then you should be able to pattern the cut-extrude feature onto your part.
I have not verified that this actually works. I abandoned that appproach for my project. Instead I created a "Block" containing the sketch entity of my cut-out shape and manually pasted that block onto my spline, everywhere that I wanted it.
Hope this helps.
Roy
Success! Mostly.
It was still a pain in the rear but not as bad as drawing 50 little circles, dimensioning them and adding 2 realationships each. The difficulty was converting the entities. Apparently, offset entities doesn't work like convert entities where you can select multiple entities. I can sort of understand why. I ended up making another linear pattern skipping the instances I needed to skip, then drawing the point sketch.
There seems to be a lot of room for improvement on patterns within sketches...
I'll probably be drilling these holes by hand though so I still need to make yet another sketch to plot out on the CNC....I suppose I could make a template on the CNC as well without much difficulty.....hmmmm...
Who'd a thunk that geometry would be useful in CAD work?