Extrude made from parametric sketch not working properly. (Possible bug?)

[Anonymous]

Being a programmer, I like being able to define models using the 'User Parameters' to generate different versions of the model by just redefining the parameters. I've done a couple of them so far, one is for square tubing where the parameters define the size of the tube and the wall thickness and another models a T-Nut.

I watched the You-Tube video by NYC_CNC  last week where he described how to model a “1-2-3” block. A “1-2-3” block is a block that is 1 inch thick, 2 inches wide, and 3 inches long. It has a rectangular pattern of holes on the face and holes that intersect these drilled through from the edges. I thought to my self, that this would be an excellent thing to model using user parameters so I set out to do so.

I created the following user parameters to use to create the model.

1. Scale = 1

2. nH_X =5 # The number of holes in the X direction

3. nH_Y =3 # The number of holes in the Y direction

4. D_Z = ((1 * scale) * 1. in) #Dimension in Z

5. D_Y = ((2 * scale) * 1. in) #Dimension in Y

6. D_X = ((3 * scale) * 1. in) #Dimension in X

7. sH = .375 in # Size for holes

8. hSpaceX = D_X / nH_X #Spacing for holes in the X direction

9. hSpaceY = D_Y / nH_Y #Spacing for holes in the Y direction

10. h1_X = hSpaceX / 2 #X of hole 1

11. h1_Y = hSpaceY / 2 #Y of hole 1

The first 3 are the ones that would be set to define the model with the rest being derived from them.

First I created a rectangle of size that had the lower left corner anchored to the origin and dimensioned it to D_X and D_Y. I then created a circle and used the “Sketch Dimension” tool to set the size and position it at h1_X and h1_Y. I then created a rectangular pattern using nH_X and nH_Y and hSpaceX and hSpaceY. I then extruded this sketch to create the block with the holes in the face.

I did a simular sketch on the left and bottom face only they only had one row of holes. I extruded them using the “Intersect” function.

I started tested it using different values for scale and nH_X and nH_Y. and it worked great until I used a value greater than 5 for nH_X or a value greater than 3 for nH_Y. When I did, it would only model that first 5 holes in X or the first 3 holes in the Y direction. Could be coincidence, but this is also the number of holes in X and Y that I had set when I first created the model.

To try to figure out what was going on I turned the sketches back on expecting to see them also missing the missing holes but to my surprise, the sketches were correct and had all the holes. Only the solid model is missing the holes.

Any ideas why the extrude is not extruding all the holes that are in the sketch? This sure seems like a bug to me.

I'm attaching some screen shots showing the model and the sketches and one of the parameters used by the first sketch and extrude.

Jody B. Caldwell

[daniel_lyall]

attach your file as well, or put a link to it from A360 it will make it easyer to find what is wrong

[Anonymous]

Sorry, I'm still kind of new to Fusion 360.  I don't know how to post the file.  Here is the link to the file.

http://a360.co/1J6m0xv

Jody

[daniel_lyall]

you need to pattern the holes not the sketch, if you delete all but your first dimensioned hole do a press pull on that hole then do your pattern from that hole use the pattern under create menu.

[Anonymous]

I understand that there is more than one way to do this, but shouldn't both methods work?  I'm not so much trying to get the model to work as I am trying to understand why the paterned sketch won't extrude properly. 

[daniel_lyall]

it's that you patterned the sketch so fusion only know to pattern that, you did the extrude after the pattern was created so changing the pattern will only change the sketch it cant add in the next function in by it's self, if you pattern the hole all that will be patterned is the holes not the sketch.

you may be able to do both at the same time never tried that idea. I might try that for fun.

[Anonymous]

No, it works fine for all cases until the number of holes is greater than 5 for X or greater than 3 for Y.

[daniel_lyall]

have you tryed to patin the hole not the sketch, when you change the sketch patin the sketches work fine i tryed 7 for x and the correct amount of sketches where there same as 5 in y all sketches where there the sketch patin worked very well. as in big words sketch patin. not extruded holes after patin was done it cant work like that. the function you did was sketch patin that is the patin only. the press pull was a second op.

when I patined the hole's it worked fine more than 5 in x and 3 in y no problems what so ever.

[Anonymous]

OK,  I've played with this some more and learned a few more things.  I've got my example simplified as much as I can and it still demonstrates what I consider to be a BUG!

First, I got rid of all my 'user parameters'.   I created a sketch with a rectangle and a 8 x 5 rectangular pattern of holes.  I then extruded that to -1 inches thick and it worked exactly as I expected.  I then went to modify parameters and just as before,  I can change the number of holes to anything I want that is less than the original 8 x 5 and it works just as I expect it to.  If  I try to do anything that is greater than 8 holes in X or 5 holes in Y it fails, just as before.  If I roll the history marker back to before the extrude and 'delete everything after the history marker' and then recreate the extrude,  it will create the extrude with the additional holes.  I recreated it with 10 holes in X.  Then, I can modify the parameters and it will work with from 1 - 10 holes in X,  but not 11. 

It will let you modify the parameters of the rectangular patter to anything less than what the extrude was originally created at, but no more.

Here is the link the the simplified version:  http://a360.co/1MgqNwl

Please look at this as a 'bug report' and not a request for another way to model the 1-2-3 block that will work.  I understand that I can 'patern the holes' and not the sketch, but that doesn't do anything to make the software better.  For that matter,  I could just make the original extrude with an outrages number of holes in X and Y and then it would work for all normal cases, but the bug would still be there.

Jody

[daniel_lyall]

I have done a screen cast showing that your sketch pattern is working so well it's not funny. and yes it can't do the press/pull by it's self it is not the operator you are.

do the thing as a hole pattern not a sketch pattern then the holes will be there just the same as a sketch pattern will be. it's as far as I know is not a bug. a pattern is a single op or a double op but you have to make the double op just like you do the single op. but you dont need to make it a double op just pattern the hole's and it will work fine.

and if you remove the circules the hole will disaper as that is what you made it do by reduceing the circule sketches.  

http://autode.sk/1Ro2iFi

  admin  your turn can you conferm if this is a bug or not or if I am that far of the mark it's not funny and will run away and cry.

[Anonymous]

If you made a screen cast, where is it?

I've already said a number of times, that I understand how to make it work by modeling the holes.  I want a file that has sketches with ALL the holes that are then extruded.  It works fine if I only reduce the number of holes from what I made the first time.  It works fine if I change the size of the rectangle.  It works fine if I change the size of the holes.  The BUG is trying to increase the number of holes beyond what was used when the extrude was first created.

[jeff_strater]

@daniel_lyall is correct here.  The problem with the "pattern the sketch" workflow is that Extrude (today at least) doesn't know that it is extruding a sketch pattern, it only knows that you extruded 15 circles (assuming 5 x 3).  It knows which 15 circles it extruded.  So, when you reduce the pattern count to, say 4 x 3, the Extrude feature goes looking for its 15 circles.  It only finds 12 of them, but those 12 it knows, so it can compute successfully.  Further, the Extrude remembers the other 3, so that if you go back and change back to 5 x 3, it finds its 15 circles, and successfully computes.

However, if you change to 5 x 4, all the Extrude knows is its 15 circles, so it doesn't go looking for any more.  From a software point of view, it's no different than if you had edited the sketch and drawn 5 more circles.  I'm pretty sure that all parametric CAD systems work this way, at least the ones that I am familiar with (although I admit I don't know every CAD systems to this level of detail).

I agree that this would be a great feature (Extrude from sketch pattern), and would be worthy of a Fusion 360 Idea Station suggestion.

In the meantime, I would recommend the workflow that Daniel suggests:  pattern at the feature level.  An added benefit is that, for large pattern counts, feature pattern is faster than sketch pattern.

Hope this helps explain how Fusion works today.

Jeff Strater (Fusion development)

[Anonymous]

Well OK then, I tried.   It doesn't seem like it should be such a complicated process to have the extrude just know that it was created from a sketch and detect when that sketch has been changed and regenerate itself from the new sketch.  If it were my software, I wouldn't want it to just silently fail and then tell people that there not supposed to actully try to use features like the sketch patern with the modify parameters thay you provide.  

Why have the sketch patern or for that matter the ability to even go back and edit a sketch at all if the downstream extrudes are just going to fail?  I just don't get it.

[roux_emler]

I'm actually in the same boat as OP is. I'm currently trying to model a rectangular insert for a utensil drawer, that I'll be making with a laser cutter and plywood. The extrusion is simply to visually double check everything will line up properly. I really only want the sketches so I can export them as DXF's and use those in a laser cutting software.

[TrippyLighting]

You responded to a truly ancient thread!

If you still need help, please create a new thread, share the model, and perhaps create a screencast.