Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Turning off retract between operations?


Guest
 Share

Recommended Posts

Hi guys,

When we are running our programs at our work, there is a return to machine Z home between operations, the spindle goes up to the max Z with an #MCS Z0, next it feeds down to the part using the tools plunge rate. If we did not detect any settings that would explain this behavior in the params or machine/control def , then is there a possibility we could fix this with post language? We need to fix this issue quickly it's costing us a lot of wasted CNC time If anyone has any Ideas what action I  should take I would so so appreciate it!!!

Thanks in advance!!

:alien:

Link to comment
Share on other sites
5 hours ago, peter ~ said:

Hi guys,

When we are running our programs at our work, there is a return to machine Z home between operations, the spindle goes up to the max Z with an #MCS Z0, next it feeds down to the part using the tools plunge rate. If we did not detect any settings that would explain this behavior in the params or machine/control def , then is there a possibility we could fix this with post language? We need to fix this issue quickly it's costing us a lot of wasted CNC time If anyone has any Ideas what action I  should take I would so so appreciate it!!!

Thanks in advance!!

:alien:

Yes, this is likely a Post issue. Typically the Post is setup to retract to Toolchange height, change the tool, then move to the XY start point (in rapid), the approach the Clearance or Retract Plane height, while enabling TLO (G43 Hxx Zzz). So the approach from Toolchange to start point should be in Rapid, unless you have "convert rapid to max feed" enabled.

Link to comment
Share on other sites
13 hours ago, Colin Gilchrist said:

Yes, this is likely a Post issue. Typically the Post is setup to retract to Toolchange height, change the tool, then move to the XY start point (in rapid), the approach the Clearance or Retract Plane height, while enabling TLO (G43 Hxx Zzz). So the approach from Toolchange to start point should be in Rapid, unless you have "convert rapid to max feed" enabled.

Hi Colin,

Thanks for the support, I checked the convert rapid to maximum feedrate is not enabled. Could you explain the TLO (G43 Hxx Zxx) or point me to a file or docs that would be relevant? I am not familiar with post language. Thanks!!

Link to comment
Share on other sites

What particular machine is this for?

TLO stands for Tool Length Offset.

In general, with a Fanuc-Style Machine, the following G-Codes are used to control positioning:

  • G00, G01, G02, G03 - Motion (Rapid, Linear, CW Arc, CCW Arc)
  • G17, G19, G18 - Planes (XY, ZX, YZ)
  • G40 / G41 / G43 - Cutter Compensation (XY Contouring Control) Programmed with a "D Value", which corresponds to the "Diameter Offset" being read for the XY adjustment.)
  • G43 / G44 / G49 - Tool Length (-,+, cancel) (Reads the "H value" to correspond to the "Height Offset" being applied to the active tool. Typically T22 = H22 = D22)
  • G54-G59 - Work Offset (XYZ location of Program Zero Point, values are typically given "in Machine Coordinates", from the Machine Home Position.)
  • G70-G89 - Canned Cycles (depending on Machine Configuration). Macros to automate repeated motion types (Drilling, Pecking, Tapping, Boring, Reaming, etc.)
  • G90 / G91 - Absolute and Incremental Motion codes
  • G93 / G94 / G95 - Feed Mode (Inverse Time, Units per Minute, Units per Revolution)
  • G98 / G99 - Controls how tools retract after a Canned Cycle Call.

Using Cutter Comp (G41/G42/G40), and TLO (G43/G49), along with Work Offsets (G54, G55, Etc.), allow us to "position a block of stock or work piece anywhere on the machine table", and then we can "tell the machine where the part is located", using a Work Offset. The Cutter Compensation (G41/G42 with a Dxx value), allow us to adjust the "XY size" of the part. We can use different "D Values" (offsets) to control different part features, allowing us to fine-tune the cutting process. TLO allows us to adjust different "depths" on the part, by making slight adjustments to different "height offsets". This allows us to compensate different "part features", by using a unique "TLO" for each feature (potentially), or adjusting "all features" that a tool cuts, by changing a single Height Offset value.

Link to comment
Share on other sites
5 minutes ago, peter ~ said:

Its is a dms 3Axis Router with a fagor 8065 controller. I believe TLO is not setup there are no H values output to the machine it only takes the tool number.

On the DMS Fagor machine, the tool offset is a single alpha-numeric, D1 if memory serves me correctly. Both height and radius are combined in combination with the #KIN (kinematic offset) parameter.

The Fagor is a very different beast from Fanuc.

  • Like 1
Link to comment
Share on other sites
2 minutes ago, So not a Guru said:

On the DMS Fagor machine, the tool offset is a single alpha-numeric, D1 if memory serves me correctly. Both height and radius are combined in combination with the #KIN (kinematic offset) parameter.

The Fagor is a very different beast from Fanuc.

Yes I am not a fan. Fanuc controllers are far Superior IMHO.

Link to comment
Share on other sites

I don't know how their 3 axis posts work but our 5 Axis DMS post uses Real Integer #8 to control mid op retracts.  If your is like this try setting #8 to 3 and see if that fixes your problem.  

And on a side note...I've been programming Fanuc and Fagor controls for 10+ years and given a choice I'll take the Fagors any day! (just my $.02 worth) 😀

image.png

Link to comment
Share on other sites
1 hour ago, jjones61 said:

I don't know how their 3 axis posts work but our 5 Axis DMS post uses Real Integer #8 to control mid op retracts.  If your is like this try setting #8 to 3 and see if that fixes your problem.  

And on a side note...I've been programming Fanuc and Fagor controls for 10+ years and given a choice I'll take the Fagors any day! (just my $.02 worth) 😀

image.png

Thank you for the info!! I will try it when I get back to the office.

Link to comment
Share on other sites
3 hours ago, peter ~ said:

My Mill page in control def looks like this -->

pic2.bmp

pic1.bmp

So it looks like your post uses Misc #1 to control retracts...I would create a couple of simple contour toolpaths, scroll down to Misc Values for each toolpath and make sure Misc #1 is actually set to 2 then post it and see what the retracts look like. I know sometimes I have to uncheck the "Automatically set to post values" box and manually change the number to make it work right, Also make sure you regenerate the toolpaths before posting them...even if they don't show up as dirty. 

 

1.gif

  • Like 1
Link to comment
Share on other sites
21 hours ago, jjones61 said:

I don't know how their 3 axis posts work but our 5 Axis DMS post uses Real Integer #8 to control mid op retracts.  If your is like this try setting #8 to 3 and see if that fixes your problem.  

And on a side note...I've been programming Fanuc and Fagor controls for 10+ years and given a choice I'll take the Fagors any day! (just my $.02 worth) 😀

image.png

That looks like a Postabiliy Engine Post.

Link to comment
Share on other sites
1 hour ago, jjones61 said:

So it looks like your post uses Misc #1 to control retracts...I would create a couple of simple contour toolpaths, scroll down to Misc Values for each toolpath and make sure Misc #1 is actually set to 2 then post it and see what the retracts look like. I know sometimes I have to uncheck the "Automatically set to post values" box and manually change the number to make it work right, Also make sure you regenerate the toolpaths before posting them...even if they don't show up as dirty. 

 

1.gif

 

Looks like the Automatically set to post values was unchecked in some Template operations. I was able to find an affected program and operation once I knew what to look for.  +1 Thank you very much  Jjones and everyone who commented!

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...