Referencing sketched hole

[hmr]

Hi Guys,

Need help

When creating a hole directly we can select a reference face instead of giving depth dimension, but while creating a sketched hole we can only select position & orientation reference faces not the depth reference. Is there any way we can reference the sketched hole depth???

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[BrianMartin]

Hi Harish...

If I'm understanding you correctly, you'd like to automatically add a reference for depth to your sketched holes. For example, let's say you sketched a hole in a 20mm thick plate and wanted it to extrude to a depth 2mm less than the thickness of that plate. There's no way to do this currently. Once you're in a sketched hole, you have no method of picking up a depth reference. You have to build that depth value into your sketch. The best thing you can do is set a sketch relation to control depth based upon other available dimensions.

For instance, you could set a sketch relation to control the hole depth based on the plate depth minus 2mm. That's about the best you can do the way the system is set up right now.

If anyone disagrees or has a better workaround, please post it because I've always struggled with this!

Thanks!

-Brian

[hmr]

Hi Brian,

You have got my point, as per you the sketched hole cannot be referenced even if we want to have depth of the hole to whole thickness of plate??

Harish

[BrianMartin]

Hi Harish...

Yep... that's what I'm saying. Even if you want the full depth, there's no way to capture that depth data other than by relation.

To use this you'd interrogate the plate thickness and note it's dimension id. Maybe you'd even rename the dimension "plate_thk" or something similar. Then you'd give your sketched hole a depth dimension. It would appear as "sd#" (for example "sd5"). You'd then write a relation in the sketcher setting sd5 = plate_thk

That's about your only option. Once you're in that sketched hole dialog box, you're prevented from picking up any additional references. The only other thing I can think of would be to create a user-defined feature (UDF) that allowed you to pick the depth reference. This would require additional work but you could then drop a sketched hole via UDF into your model and reference a surface to pick up the depth.

I wish I had a better answer for you. I think this is about the best we have!

Thanks!

-Brian

[hmr]

Thanks Brian

[KrisR]

Typically the "first" extruision in a sketch has a depth value of "d0" (that is a zero). As I make subsequent holes that I want completely thru,, I'll use "d0" as a relation in the value box and then add the relation.

[hmr]

Thanks Kris, That't what even Brian was advising but my requirement was to reference the depth of sketched hole for which I couldn't get solution.

[TomD.inPDX]

You can always do a revolved cut with a sketch instead of a hole feature. Then you can use relations and/or references.

What about UDF's?

[hmr]

Hi Antonius,

Yup, revolve is one more option which i can give a try for, Sketched hole is also revolve itself, except that there is no option to select references in sketched hole right???

I have not created any UDFs, Advice me some good material to go through & try some, please.

Best Regards,

Harish

[TomD.inPDX]

http://learningexchange.ptc.com/tutorial/464/creating-udfs

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[hmr]

Thank you