Curve 5X MultiPass Retract

[khass0410]

Hi everyone,

Hoping yall can help me figure out if i'm doing something wrong or if it's my post or if I need a post modification.

I’m using the toolpath Curve 5 Axis with two passes in multi-pass. For every pass it makes the tool goes home in Z “G0 G28 G91 Z0.”. Is it suppose to go home for every pass? I would think that if “Keep tool down” is not checked the tool would retract to its clearance plane and reposition for lead in and out and if “Keep tool down” is checked it would not retract to its clearance plane but stay down and reposition itself and carry on. If you open up the attached output you will see the tool going home around line 359.

 

The attached file has 3 toolpaths within it… The 1^st Operation has keep tool down checked, the 2^nd Operation does not. The 3^rd operation is in a different tool group and is for the pocket on the opposite side so I would expect if Operation 2 and 3 were posted out together for the tool to go home before moving to Operation 3.

 

I am also using Swarf Milling, Morph, & Multi-axis Rough with multi-passes and depth of cuts and these toolpaths do not go home until they transition to another pocket. Thanks for the help.

CURVE_5X_TOOL_RETRACT.mcam

KEEP TOOL DOWN OFF.MIN

KEEP TOOL DOWN ON.MIN

[crazy^millman]

On 4/23/2020 at 12:51 PM, khass0410 said:

Hi everyone,

Hoping yall can help me figure out if i'm doing something wrong or if it's my post or if I need a post modification.

I’m using the toolpath Curve 5 Axis with two passes in multi-pass. For every pass it makes the tool goes home in Z “G0 G28 G91 Z0.”. Is it suppose to go home for every pass? I would think that if “Keep tool down” is not checked the tool would retract to its clearance plane and reposition for lead in and out and if “Keep tool down” is checked it would not retract to its clearance plane but stay down and reposition itself and carry on. If you open up the attached output you will see the tool going home around line 359.

 

 

 

The attached file has 3 toolpaths within it… The 1^st Operation has keep tool down checked, the 2^nd Operation does not. The 3^rd operation is in a different tool group and is for the pocket on the opposite side so I would expect if Operation 2 and 3 were posted out together for the tool to go home before moving to Operation 3.

 

 

 

I am also using Swarf Milling, Morph, & Multi-axis Rough with multi-passes and depth of cuts and these toolpaths do not go home until they transition to another pocket. Thanks for the help.

CURVE_5X_TOOL_RETRACT.mcam

KEEP TOOL DOWN OFF.MIN

KEEP TOOL DOWN ON.MIN

Go to the linking area and look at Safety zone. there is bug when adding them after a toolpath is created. You need to create them as your making the toolpath. It will only allow 3 shapes. I would look to Cylinder and that should solve your issue.

Pic1

Pic 2

 

 

[crazy^millman]

I seen your surfaces in the file, but not a dumbed down solid. I use Model prep and dumb solids down for what you're doing with the surfaces. Make creating toolpaths that much faster and easier without all the extra cad your creating for the surfaces.

One with the ID and one without.

Pic 3

Pic 4

[khass0410]

1 hour ago, 5th Axis CGI said:

Go to the linking area and look at Safety zone. there is bug when adding them after a toolpath is created. You need to create them as your making the toolpath. It will only allow 3 shapes. I would look to Cylinder and that should solve your issue.

 

 

 

So I tried creating a new curve 5 axis toolpath with the Safety Zone and I'm receiving the same code as I was before with the tool returning to Z0 before making the second pass. So maybe it's my post? Or my post is ignoring the safety zone? I agree about the dumb downed solid I do have one but didn't create my toolpaths off of it. The file I sent was just a small bit of what I have in it. Thank you for the help.

[gcode]

Is this a Postability post?

If so check out the Misc page 

There are 2 fields, lower right that control retract behavior

By default they are 0, change them to 3

If it's not a Postabilty post, check the Misc page anyway.

Look for a Safe Retract switch and turn it off

 

 

[khass0410]

17 minutes ago, gcode said:

Is this a Postability post?

If so check out the Misc page 

There are 2 fields, lower right that control retract behavior

By default they are 0, change them to 3

If it's not a Postabilty post, check the Misc page anyway.

Look for a Safe Retract switch and turn it off

 

 

This is a MLC post, so my Misc. Values page is a little different. My MR6 is a Safe Z Retract and when I turn it to None it does keep the tool down during multi-passes but say I'm doing more then 1 pocket when the tool is done with the 1st pocket the tool won't return home it stays down because the Safe Z Retract is set to None.

[gcode]

Have you tried putting a value in MR1

[khass0410]

8 minutes ago, gcode said:

Have you tried putting a value in MR1

I just tried that after you mentioned it and nothing happened. So if I remember correctly MR1 in the post is based off of MR6, If MR6 is disabled in the post it will look at MR1 and apply it to all toolpaths.

[crazy^millman]

This is a post related issue and might need talk to them about getting a better post or added ability to your post. 

[khass0410]

7 minutes ago, 5th Axis CGI said:

This is a post related issue and might need talk to them about getting a better post or added ability to your post. 

Ron, Thank you. This is what I was needing. I've been in contact with my reseller. Just wanting to make sure that it was a post related problem. Hopefully they can fix me up.

Ron do you mind me emailing you about something you helped me with in another topic?

[crazy^millman]

2 minutes ago, khass0410 said:

Ron, Thank you. This is what I was needing. I've been in contact with my reseller. Just wanting to make sure that it was a post related problem. Hopefully they can fix me up.

Ron do you mind me emailing you about something you helped me with in another topic?

No problem you have my email.