Problems with parameters

[jake.mansfield5FA56]

Hi Guys,

I have created a sketch using parameters so i can easily change a job we do without having to re draw. Every other variable seems to work fine except my repeats parameter.

I am using the repeat parameter in a rectangular pattern hence why it has no unit. I'm using it for the 'Quantity' in the rectangular pattern as some parts have more holes in than others. 

This worked fine up until i came to change that parameter

this is how my part looks before changing this parameter (the rectangular pattern is for the cross holes in the cylinder)

but as soon as i change this particular parameter, it turns my model into this??? 

i have no idea why it is doing this as the parameter should only change the number of times the cross hole is repeated?? 

please help?! 

Thanks 

[TheCADWhisperer]

Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

Edit:  Can you Attach your part in the failed state that you show in image?

[jake.mansfield5FA56]

Here you go, 

Thanks

[TheCADWhisperer]

Why the repeated workplanes?

Why the repeated sketches?

I recommend that you use Feature (or Face) Patterns, not sketch element patterns. 

(And not repeat work. I feel like I must be missing something with the Design Intent?)

[ritste20]

I'm still reviewing your model but one thing to consider as a general rule of thumb: it's better to pattern features than sketch entities whenever possible. The less you need to modify sketch elements whether by parameter or physical edits the better, hands down.

Regards,

[jake.mansfield5FA56]

I am a fusion noddy 

[jake.mansfield5FA56]

the reason i done it on sketch is its just how ive always done it. is it better to do in solid then?? 

[TheCADWhisperer]

@jake.mansfield5FA56 

Diametral dimension.

and use Feature Pattern...

...don't duplicate work.

See Attached.

[johnsonshiue]

Hi Jake,

I took a quick look at your design. I think I know why change of "Repeat" leads to drastic change in shape. The issue is with the profiles to cut in the last four Extrusions. When "Repeat" reduces its value, the number of profiles is reduced. Your design intent is to have fewer holes. However, the Extrusion cut still remembers the profiles to cut. Instead of drilling the holes, the rectangular boundary is also selected as a cut profile. As a result, the rod becomes rectangular as opposed to circular.

The behavior is somewhat expected. It is because the Extrusion feature isn't aware that only the small circular profiles need to be kept, and the newly added circular profiles need to be included. Such intelligence does not exist.

Like other experts already suggested, I would pattern the feature instead of patterning the sketch. You will be able to control the number of pattern instances. The drawback of patterning sketch geometry is that you cannot control which profiles to be selected or unselected when the pattern changes.

Many thanks!