Yeah, another Array/Pattern problem

[BillB]

Hello Folks,

 

As seen in the attached pic, I am trying to Pattern the cut/extrusion along the front surface of this "thing". I've looked in J.D.'s MA105-1 tutorial manual and have tried various different methods without much luck.The "cut" was made as a separate extrusion in the curved part if this is of any interest. This isn't a high accurate piece at this time but will probably evolve into one later on. Anybody have any suggestions or comments on this

 

Thanks for any help in advance, have a good one.

 

BillB

[Dana W]

Do you have arcs that you can array equidistant (radial) lines along?

Maybe you could then mirror the extrusion along the surface using the arrayed lines as mirror lines.

[kencaz]

Try a 3D sketch "include geometry" the edge of your spline for use as a path for the array...

 

KC

[BillB]

Hey Dana & KC

 

Thanks for the response guys. KC, what you suggested seems to work pretty good, thanks. Haven't used 3D Sketch much at all yet, but that seemed painless. I am going to start tweeking it and see where it may lead me. Thanks again and take care.

 

BillB

[shift1313]

is your part not planar? If it is planar you could do the same thing with a 2d sketch as well. I just did the same thing but created a new sketch specifically for the path(see image). You could also share the sketch used to create your original part or select the edge for your path in a rectangular pattern.

[BillB]

Hey Matt,

 

Man,,, I hate to admit it,, but what you just said went over my head, sorry. The front face is made up of three tangent radius's and although I can get these 12 or 13 "teeth" to follow along the path of 3D Sketch per KC's suggestion, I still have 1 or 2 that won't completely cut clean at the top of the "tooth" valley. Hope this make since.

 

BillB

[shift1313]

the planar comment, i was just asking if the side faces were flat. So basically you drew that part and extruded it so the path your cuts will follow is in 2d.

 

Do you need the pattern to be 12 equally spaced or do you need a certain spacing and as many as you can get? there are options when performing a linear pattern for this type of thing.

 

can you post a screen shot of the 2 that wont cut clean?

[BillB]

Hey Again Matt,

 

Yeah,, sorry. The sides are flat to one another and perpendicular to the front and back surfaces (front surface being the one that's getting the "teeth" cut into it.) Here's a pic of how far I've got so far. This "thing" is going to be a prototype cut from steel (laser or plasma) that I had to draw from a "carved/cut" wooden piece that some log jockey brought in, get the idea?

 

Thanks for the help Matt, I do appreciate it.

[JD Mather]

Rectangular Pattern can also be used as "curve driven pattern" . See the AU tutorials in my signature.

[shift1313]

the problem is your cut out is actually below the surface meaning the curve you are following is probably going through some negative curvature there because up until that point it was arcing away from the cut. You can solve this by making your cutout larger. Ill try to take some screen shots later on tonight if you havent got it(or someone else chimes in)

[shift1313]

Here are a few screen shots for you bill. The first thing I did was draw your shape with a single spline using only the end points handles to control the shape. What this does is lets me select the edge of my solid as my direction for the pattern without having the addition of any other sketches. creating the shape with a bunch of arcs, even though they are tangent, will produce those separated faces.

 

Special note on how i created the cut out. I created a line from spline to spline, then a second line that was perpendicular with that one. This perpendicular line then got a tangent constraint with the spline. This is important so that your cut outs orientation is not only right for the first one, but as it travels along the path.

 

In the 3rd image you can see the red line selected as the direction.

 

Also note in the 4th image the orientation button is selected as Direction 1. This will adjust the cutout along the spline. There are limitations to this depending on your cutout and the radius you are trying to bend it around.

[pinco pallino]

Hi folks

not long ago I experienced the same thing on a circular pattern.

Today I tried BillB's work and found the same problem. (see pics. the curve is a coplanar spline here)

I used a rectangular pattern as JD suggested and extended the cut, out of the curved surface. As Shift pointed out, I too, thought that was the issue but the result didn't change.

I tried a rebuild all and no difference

Shift u asked if the surfaces were coplanar. Do u mean that the pattern could follow an irregular 3D surface?

I know it follows spirals but I never tried an irregular 3D surface. Also u mentioned incremental spacing, I tried that some time back with no success.

I'd like to find some more about those two

cheers

Ralf

[pinco pallino]

I checked the Adjust button under Compute and that did the trick.

[BillB]

Matt, J.D. & Ralf,

 

Thank you all for the great input. I'll give it another try in a short while, updating another job at the moment. I'll let you know one way or another. Thanks again guys, have a great day.

 

BillB