Heights Tab

[gussycool1]

New to the forum and fusion

Need some assistance on using the heights tab. I set up for drilling multiple parts in a fixture and crashed into the fixture moving to the next part after the first drilled part. My question is : After the drill cycle is completed and moves to the next part, does it rapid from the feed height or the retract height. When I Simulated the operation there was no collision in simulation assuming then it was good.

A few facts is that I set feed height .250 above hole -retract and clearance height was set above fixture.

Thanks

[seth.madore]

Is your Fixture modeled up in your file? Can you share a bit more info, such as machine and post processor being used, perhaps your Fusion file (If it contains linked components, those will need to be broken)?

File > Export > Save to local folder. Return to thread and attach the .f3d file in your reply. If you'd rather not make your design public, you could PM me the a360 link

[gussycool1]

DON'T HAVE AN OPTION IN THE EXPORT FILE FOR .f3d file

[gussycool1]

I used a generic post and did alot of pass through which I find interesting in Fusion

been a Surfcam user for a number of years and there was able to edit the post.

This program was to run on an Allen Bradley 8400 control.

Thanks

[seth.madore]

There is no post in Fusion or the HSM Post library for an Allen Bradley, but I did find THIS POST here. Give that one a shot?

In your CAM  history, you got a lot of stuff going on. Where exactly is the problem?

Are we looking at the actual fixture being used, or is this the end product in it's assembled environment?

In some of your drilling cycles, you are drilling angled holes, but you don't have "Tool Orientation" enabled, which will certainly give you problems with Heights and g-code.

[gussycool1]

Thanks for your response. I will attach the post processor that I used but pretty much had to edit it and of

course use the pass through to aid for output. As far as tool orientation I rotated the table + 7 deg

and then -7 deg . Did tool-path for each angle separately and then protected it. This way I could keep fixture offset the same. Little unorthodox but it seemed to work. The original question was in moving to the next drill cycle (hole) does

Fusion use feed height or retract height. I mentioned earlier with simulate it showed no errors.

Appreciate the support

[gussycool1]

attached is the post I used but also edited the g-code and also used pass
through to help in running the program. If you like I can send you a sample
of the edited program and proper layout for an Allen Bradley 8400 MP. I
owed one for 10 years and had a post designed thru post haste
in Surfcam. I'm new to Fusion As I mentioned earlier and wanted to thank
you for all the help.

[seth.madore]

---

@gussycool1 wrote:

The original question was in moving to the next drill cycle (hole) does

Fusion use feed height or retract height. I mentioned earlier with simulate it showed no errors.

Appreciate the support

---

Looking at your post and what it outputs, it is possible that this format is not correct for your machine.

S2290 M3
G0 X0. Y0.
G0 Z1.
G81 X0. Y0. Z-0.8 R0.05 F23.
X-0.6716 Y-0.5528
G80
G0 Z1.

Does your machine support G98 and G99/G98 will retract to Clearance/Retract plane (they can be the same value) and G99 will retract to Feed Height.

At any rate, you can see that the first hole is drilled: G81 X0. Y0. Z-0.8 R0.05 F23.

And then it moves over to the next hole. At no point does it move back to the safe plane of 1" above part.

So, how does your machine WANT to see the code to retract safely?

Where did you get this post; a modification of your own design, or from that thread that I referenced earlier in the post?

[gussycool1]

Hi,
the post was derived from a Allen Bradly post thread but was missing some
basic codes-So I added the pass through-thru out the program to generate
the post output.
G99 is used as" Cancel Presets" that will not work as this clears modal
codes . I would have to look at manual for the G98. I could run a sample
thru my post processor in Surfcam to see an output.
Question- where would you put the G98 in the code since I would have to
manually do it anyway.
Many thanks
this has been exhausting.
FYI--Owner does not want to spring for a custom post. Why not !!

[seth.madore · Accepted solution]

Well, if the machine/control are nearing obsolescence, I can sort of see his point. Even still, the time spent hacking around and whatnot will soon exceed the cost of getting something proper...

The other option would be to have Fusion post out long hand code. It's not going to be friendly on code size, just as a warning...

According to THIS manual, it looks like G92 might be the answer needed: