Transfering a hole(pattern) from one part to another.

[steamwise]

Having drawn a pattern of holes on an irregular shaped cylinder head, I want to transfer the hole pattern onto the cylinder block. Is there an easy way to do this on on the assembly? Is it possible to sketch out the holes and then extrude cut through both parts mated in an assembly? I have spent many frustrating hours trying to get this to work, it seems so obvious a function, but I am missing the plot somewhere! Hope someone can help.

Thanks

 

Mike

[JD Mather]

Edit the block in the context of the assembly.

Start a new sketch.

Convert Entities the circles from the holes of the head.

You probably want to use these to locate tapped holes using the Hole Wizard rather than Extrude - Cut (the tapped holes are smaller tap drill size than the through clearance holes in the head).

[bhamze]

I would create a sketch as reference geometry (hole pattern) inside the assembly. Click on sketch in feature tree then select insert/assembly feature/cut/extrude. In the cut-extrude dialog box you will have a feature scope option, here is where you select what part gets the cut feature. There are other ways but this is the easiest.

[shift1313]

Another method would be inside your head/hole pattern sketch, go to your Tools>Blocks menu and make a block of this fully defined sketch. Then got to Tools>Blocks>Save Block and save this in a location you know. Then when creating your cylinder, inside a sketch you can insert this block. I do this all the time for things like circuit cards, connector openings and so on.

 

The best method is probably to draw both the head and cylinder in a single part file as separate bodies(merge results check box when creating features). Like bill mentioned you can select the feature scope for which you want to extrude/cut and you can always convert entities, or even simply draw a circle and make it concentric to the hole in your head. If you create multi body parts you can expand the solid bodies folder in your feature tree, right click on one of the solid bodies(at a time) and use "Insert into new part". As long as you dont break the reference, these new part files will update whenever you go back and change the original part file.

[steamwise]

Thanks Guys,

 

I'll give all these a go. As I said, I have struggled with this for some time so I am glad it is not as straight forward -to a novice - as I expected it should be.

 

Mike

[steamwise]

Taking the question one step further, can any of you guys suggest a way of transfering an existing pattern of holes in an already created part, onto another 'blank' part in an assembly. The attached picture show a cylinder mounted on a boiler barrell. The holes in the mounting saddle have already been created. So... how can I get this pattern onto the barrell without having to re-draw everything.

 

Thanks for everything,

 

Mike