CAM: Drilling, set clearance height as 'move to' before next hole

[Coscor_NPL]

Hi all

This one is relativly simple

When I drill below scenario, I would like to be able to move the drill to clearance height after each boring in a cycle

As you see on picture below, the tool moves through my 'clamping equipment' what I need is a box to 'tick' to tell that it should:

'retract to clearance level after each finished boring'

Thanks for listening! if, you need any more info please let me know...

[Laurens-3DTechDraw]

What the system is doing is the following(Not all machine cycles do this so your post might cause other things to happen):

1. Move to clearance height and XY of first hole. (Rapid)
2. Move to retract height. (Rapid)
3. Move to feed height. (Rapid)
4. Move to top. (Feed)
5. Drill the hole (Feed and possibly pecking, or a boring routine)
6. After dill is done move to hole top.(Rapid)
7. Move to retract height. (Rapid)
8. Move to XY of new hole. (Rapid)
9. Move down to feed height. (Rapid)
10. Drill the next hole.

So your retract height is the one you would need to set above your clamps and you are good to go.

[HughesTooling]

If you want the clearance and retract the same just set them both to Model top + 95.

Mark

[Coscor_NPL]

Hi both

Thanks for the 'tip'

You are correct, I can see that this is how it works in the simulation

The problem is that not all machines/softwares support this, this means that this does not work on (as in my example) on Heidenhain530 (this is not ancient/hobby machine software) software/machine. what happens if I do this on my machine with a 'correct' post is that it uses feed all the way from the retract to 0 for the first chip...

Stupid i know, but it is defiently not unusual, only way to fix this for me is to change the post to manually move to clearance after each boring, (after the M99) and keep the retract where it should be (5mm over part top) in F360.

The problem with this is that then I cannot rely on the simulation/toolpath in fusion 360 and I do not have the easy option to disable this sometimes timeconsuming high retract (see picture below) (I manually imputtet the z+80 for example)

This is 'easy' for the 360 team to fix, and would mean a lot for many people, with a simple 'tick to move to clearance after each boring' many CAM softwares have this option.

Don't get me wrong, I appreciate your answers. Just if I understand it will not fix the problem in a good way

Thanks. 

[HughesTooling]

A postprocessor could be made so that if you set the Clearance and Retract to the same height a rapid to the retract is output at every hole. I think the posts are done so they are as safe as possible so it might be slow but you're not going to run into the clamps.

It might be worth putting a request in the CAM post form. HERE. Even if a move to clearance option was added to the dialog the posts would need the same mod to make it happen.

Mark

[Laurens-3DTechDraw]

On your Heidenhain iTNC 530 I would suggest using the 205 cycle instead.

Why did you modifiy the post to output Cycle 1.0? I mean that's not standard right?

The post is set-up to support cycle 205 with a very easy change.

[Coscor_NPL]

Hi

HughesTooling -> actually your last comment gave me an idea, I could change the post processor, so I could make a 'custom variable' (like the blue line on picture below) so the posted file go to clearance after each M99 (cycle call) or something like that.... then i could enable this when I know there are high clamps etc. to 'deliberately cheat'

Laurens-3DTechDraw -> I must admit I have never heard or used a cycle 205... all my post processors have never used this, and are not sure it is included/supported by the the machine... But why shouldn't it? I will for sure check this cycle out when I get to my machine! Thanks! looking forward to check this out!