topic Re: Subprogram for z height changes in Fusion Manufacture Forum

Subprogram for z height changes

jdkendall97 — Thu, 21 Dec 2023 17:04:15 GMT

Hi,

I have an older control with limited memory. And I am trying a high feed mill for the first time. My Y travel is used to the max so i cant do straight moves so I need to find a way to have the z height called and the x and y moves be a subprogram. How do i do this?

Re: Subprogram for z height changes

seth.madore — Thu, 21 Dec 2023 19:35:04 GMT

How "Limited" is your memory on the controller?

Re: Subprogram for z height changes

jdkendall97 — Thu, 21 Dec 2023 20:26:12 GMT

About 25kB

Re: Subprogram for z height changes

seth.madore — Thu, 21 Dec 2023 20:36:49 GMT

And what post processor are you using?

Re: Subprogram for z height changes

seth.madore — Thu, 21 Dec 2023 20:52:44 GMT

So here's what I recommend:
Create a toolpath at a single Z level (your starting height Z level). Place that toolpath into a Linear Pattern, with the direction being your Z axis and your increment value being your depth of cut. Specify the number of repeats.

Using a post processor that spits out Sub program files, set it to "Patterns".

The result looks something like this:

(view in My Videos)

Re: Subprogram for z height changes

jdkendall97 — Tue, 26 Dec 2023 21:26:50 GMT

To answer your question, I have an okuma post I modified. I did watched your video and tried it out. It looks like it is not retracting the model top on the subsequence moves and is going to hit the part on some of the moves. To fix that I separated out those to see if it would lift up but it did not. I cant make it do long paths to avoid hitting the side of the parts because it is at the limit of the y travel. However it did significantly reduce the program size.

Re: Subprogram for z height changes

jdkendall97 — Wed, 27 Dec 2023 18:56:14 GMT

Is there a way to make it fully retract to the model top plane every time to not hit the parts?

Re: Subprogram for z height changes

seth.madore — Wed, 27 Dec 2023 19:21:28 GMT

Yes. Use a Manual NC command with a Passthrough snippet of code "G0G90Z.5"

The result will be this for the main code:

(FACE SIDES) G00X0.23Y9.025 Z1.23 M98 P1002 G0G90Z.5 (FACE SIDES) G00X0.23Y9.025 Z1.19 M98 P1002 G0G90Z.5

And the subroutine will still be the same as it was prior.