using parameters

[Anonymous]

Hi,

I have created a disc which is 300mm external diameter and 200mm internal diameter, also I have added 12 pockets which are 9.55mm wide by 12.0mm long on a 220mm pitch circle diameter, all extruded to 8.0mm thickness. I have successfully created parameters for the 300mm dia, 200mm dia, 8.0mm thichness and the number of pockets (12). When I change the values for these features the model changes accordingly. I then added the width and length of the pockets 9.55mm and 12mm respectively to the parameter list in the same way, the system accepts the inputs but fails to change the size of the pockets in the model. What am I doing wrong?

jj

[jeff_strater]

Hi JJ,

Thanks for the post.  I think I understand your questions, but it is a bit hard to tell what is going wrong without some more info.  Would it be possible to share your design?  Or at least an image and some additional description?  For the length and width of the pockets, are you using a sketch to create the pocket, or a primitive?  How did you hook up the parameters to the length and width?

We'll be happy to help figure this out.

Jeff Strater (Fusion development)

[Anonymous]

Hi Jeff,

How do I share this drawing with you?

jj

[Anonymous]

Hi Jeff,

Thanks for the reply, the 12 pockets have a 3.0mm fillet in the 4 corners of each pocket. I have just added that parameter to the list, when a new value is input into this parameter it changes not only the fillet radii but also the width and length of the pockets. So the fillet and the pocket width and length are some how dependent on each other. When the sketch was created I used the centre rectangle tab, then added the fillets into each corner. Then a circular pattern to create the other 11 pockets. I am at a loss why I cannot alter just the width or length of the pockets using the parameter list. Must I redraw the model using a different method for this design?

jj

ps. I have added an image of the disc

[jeff_strater · Accepted solution]

Ah, thank you.  Great explanation.  I understand now.  Here's the problem (and yes, it is a Fusion bug):

When you added the fillets, the dimensions that created the pocket got broken.  It's a known problem with sketch fillet.

When you created the rectangle, the dimensions were between the endpoints of the line:

but, when the fillet was added, it broke the relationship - the dimension still exists, but to points that are in space:

There are two ways you can fix this:

1. delete the dimensions and re-create them between the pairs of parallel lines, not the line endpoints:

This is probably the easiest workaround

2. you can add coincident constraints between those points and the rectangle lines:

This is more work, IMO.

It is fair to expect Fusion to handle this itself.  It is a known bug, and is being worked on, but is not fixed yet.

Hope this helps,

Jeff

[Anonymous]

 Hi Jeff,

Thanks for the help, the fix looks fairly straight forward.

jj