topic Re: Need help understanding two sided machining in Fusion Manufacture Forum

Need help understanding two sided machining

t.g.mandel — Wed, 24 May 2023 15:23:45 GMT

I am working on my first two sided 3D project, have read and watched many tutorials on the subject, but unfortunately feel I am not understanding the process.

I am trying the 'pin/dowel' method, and to date have:

1. Finished the CAD and CAM for the first side

2. Have included two 6 mm dowel holes in the design

3. Have machined the two dowel holes in the 1st/top side of the stock, as well as the spoil board

4. Have tested/machined the tool paths for the top side

*5. When I set up the bottom side with one test tool path and new WCS, it does not look correct to me and this is where I would appreciate guidance. I am still experimenting with all processes for this project, so if I have made a fundamental error I will not have lost any important material etc, and will be happy to learn from my mistake.

Here are some images to help understand the project:

The top set up

The bottom set up and first test tool path

The project before flipping onto the dowel pins - note I flipped it over to the right/x axis

Here is the position of the end mill before the start of the bottom tool path (I raised the Z height a little for the picture). The position seems off to me given what I was expecting after flipping the stock onto the locating pins, hence why I feel I need help.

I have attached the CAD/CAM file.

Re: Need help understanding two sided machining

seth.madore — Wed, 24 May 2023 15:37:53 GMT

Whenever I am locating parts on dowel pins, I try to make my origin the center of that hole, both at the machine and in my Fusion WCS settings. Your WCS Z can either be set on the spoil board or the top of the stock. But, X and Y are better placed at the pin (since it's a known location in Fusion).

For it to work in the manner that you've done it, would require that the dowel holes be equally spaced along the X axis, with identical values from one hole to the edge and from the other hole to the opposite edge.

Or, just use a dowel location as your X/Y 🙂

Re: Need help understanding two sided machining

t.g.mandel — Wed, 24 May 2023 15:53:45 GMT

Thank you, that is what I thought after I saw where the bottom was showing the X/Y zero - see image below:

It seemed off to me, and given your explanation, by about the difference the pins are set in from the two sides. I am happy to start again, but given I am also testing my two sided tool paths - checking for clearances, z heights, and how the tabs will function - is there a creative (mathematical) way for me to still salvage this set up, so that the top and bottom toolpaths still align?

Re: Need help understanding two sided machining

t.g.mandel — Wed, 24 May 2023 16:16:53 GMT

Here is my idea.

I am not sure if you noticed my 'learning opportunity' in the stock? It is the scorched circle where my end mill and ISO20 toolholder crashed into the material - I used a new tool for the previous operation that I had not calculated the offset for in my tool table...lesson learned.

Since the end mill went through the bottom, could I use my 3D probe to find the centre of that hole - it is one of the dowel pins - then change my bottom set up to use this point as my X/Y centre? I had surfaced the stock, so am confident of the Z height to use.

Or alternatively, use calipers to measure the distance from the stock sides to the dowel hole centres and calculate the offset needed?

As an aside, is there a way to get the stock as a sketch for use in determining dimensions/distances between it and the model? It disappears when I try to use the measure feature to see how far the holes are from the stock edges.

Could either work to get me close?

Re: Need help understanding two sided machining

seth.madore — Wed, 24 May 2023 16:27:37 GMT

@t.g.mandel wrote:

Here is my idea.

Since the end mill went through the bottom, could I use my 3D probe to find the centre of that hole - it is one of the dowel pins - then change my bottom set up to use this point as my X/Y centre? I had surfaced the stock, so am confident of the Z height to use.

Yep, that's exactly what I would do! When I put dowel holes in parts, I always try to get them to be "thru holes" so I have something to probe on. If that's not an option, I find another feature I can machine thru and then probe.

For your Stock/Measurement issue; you would need to have the stock defined as a Solid Model and then select that stock in your Setup.

Re: Need help understanding two sided machining

t.g.mandel — Wed, 24 May 2023 16:45:43 GMT

Thank you for your continued support - I appreciate it.

I had yet another idea, if for example I did not have a probe, that I thought could work:

Run my dowel operation, but stop it when it is just about to re-machine the first hole location.

I find the machine coordinates, and I choose a new G** offset and set this position to X/Y zero.

Then in my bottom setup, I make the centre of this hole my WCS X/Y zero, and regenerate my tool path(s).

Is this also a viable solution?

Re: Need help understanding two sided machining

seth.madore — Wed, 24 May 2023 17:11:44 GMT

Yep. Another method (if your control supports it) is to look at the code, write down the XY position and in MDI, have your machine move to that spot (based on your 1st op work offset). You then store that current position in your next work offset.

Re: Need help understanding two sided machining

t.g.mandel — Wed, 24 May 2023 21:51:08 GMT

It worked, and both sides lined up perfectly using the latter method of having the dowel hole centre as the new X/Y zero reference - thank you again.