Boring an Internal Hole

[chrisjh777]

OK, show me how to bore this simple hole using HSMWorks Turning.
 
Here are the conditions:

There is a clearance hole Φ25 for the boring bar to enter.
My custom boring bar is set up Left Handed, and I run the spindle in Reverse (M4).
The finished size is Φ40.1mm x 20mm deep.
Stock is Φ50mm.
Datum is Centreline at the Face of the Stock.

Boring Bar is setup as shown in the attachment below:

All I get if I select “Machine Inside” is shown in the "Error Message" attachment below:

I have attached a Solidworks Assembly containing both the part to be machined and my boring bar.

Can someone upload a YouTube video demonstrating that HSMWorks internal boring actually works?  I can't find one video anywhere demonstrating Internal Boring.

[Laurens-3DTechDraw]

Chris Humphris wrote:

OK, show me how to bore this simple hole using HSMWorks Turning.   Here are the conditions: There is a clearance hole Φ25 for the boring bar to enter. My custom boring bar is set up Left Handed, and I run the spindle in Reverse (M4). The finished size is Φ40.1mm x 20mm deep. Stock is Φ50mm. Datum is Centreline at the Face of the Stock. Boring Bar is setup as shown in the attachment below: All I get if I select “Machine Inside” is shown in the "Error Message" attachment below: I have attached a Solidworks Assembly containing both the part to be machined and my boring bar. Can someone upload a YouTube video demonstrating that HSMWorks internal boring actually works?  I can't find one video anywhere demonstrating Internal Boring.

Without the parts that are in the assembly not much we can do.

[chrisjh777]

Sorry,  Attached are the models of the part + the boring bar + Insert.

[chrisjh777]

OK,  I am an amateur.

Here is a Solidworks Pack and Go Zip File.

[Laurens-3DTechDraw]

Problem is your tool isn't set to M4.
Do that and it works.
I also changed your confinement because I never like the tool to start inside the model.

[chrisjh777]

Hi,

Thank you 🙂

I use a gang tooling setup and use the same LH boring bar to OD and ID turning.  This means I need M3 for OD Turning and M4 for ID Turning.  So I now have set up the same tool twice, one with M3 and one with M4.

Question:  I am using SW2015 SP4.  Can I use HSMworks 16 with SW15?

Regards

[Laurens-3DTechDraw]

Chris Humphris wrote:
Question:  I am using SW2015 SP4.  Can I use HSMworks 16 with SW15?

Yes, up to three versions back.

[chrisjh777]

OK,

My machine uses a Gang Tooling arrangement where some operations (including boring and parting) are performed at the rear side of the centreline.

Try as I may, I could not choose values in the radii tab to generate a toolpath on the rear (negative side) of the centreline.  I tried all sorts of combinations of negative radii.

Eventually I got around the problem by generating positive values of X (as if the tool tip was in a RH Boring Bar), posting the code, then hand editing the code in a text editor.  I did this with a global search and replace i.e. "Replace all occurrences of X with X-".

I also had to add by hand a withdraw from bore move as HSMWorks left the tool inside the bore.  This was done with a simple G00 Z20 at the end of the code.

This worked for me.

Unless I am mistaken, HSMWorks turning cannot handle tool paths on the rear (negative) side of the centreline.

[chrisjh777]

Hi Lonny,

Thank you confirming my observations.  I was beginning to think my aging brain was letting me down.

Having used my gang tooling machine for some time now, I am aware of the reversed arcs.

Regards

[tacticalkeychains]

I turn on the - side for parting off, as I use Gang Tool aswell this saves about 4" of table space. I run my turning tools upside down, so the part off is still "right side up"  It took a post edit, what control do you have, fanuc or fagor maybe?

[chrisjh777]

TacticalKeychains wrote:
I turn on the - side for parting off, as I use Gang Tool aswell this saves about 4" of table space. I run my turning tools upside down, so the part off is still "right side up"  It took a post edit, what control do you have, fanuc or fagor maybe?

I use Mach3 as the controller on my home made CNC Lathe.  No fancy expensive controllers here. Mach3 responds well to Generic Fanuc commands.

So what I do is post to a Generic Fanuc post processor, and then hand edit the posted code to remove code that Mach3 does not need (or in this case, change the positive X values to negative).  I then copy the amended code and paste into my own proven templates (or, more often, paste into a copy of a program I have used previously). 

Some more hand editing (principally on the start and end of the program) and I have code that I can use.

For any threading (external or internal) I hand amend previous G76 code to suit the thread pitch, diameter and length) and insert the code into the program.

For tool calls, I use G52 offsets for each tool.  Works great.

I have attached a copy of the code I produced last night for this boring operation.

I have a few YouTube videos of my CNC Gang Tool Lathe in action.  Just search for chrisjh777 on YouTube.

[tacticalkeychains]

That sounds terrible, in this case it would need extensive post edits, or just hand code. Hand coding a lathe is very simple for any of the parts I have done (except radii, for that I just tumble the part, haha) Have you tried the "slant pro" post? It's for pathpilot, but for the Tormach I now have path pilot, but my mach 3 tormach post works with path pilot, so figured it is backwards compatible.

Another person to talk to would be one2tencnc on YouTube/instagram  he has a home built rig running mach 3

[chrisjh777]

OK. My code worked fine. 

Just completed a batch of 20 PVC parts using my modified boring routine, and a standard unmodified HSMWorks generated OD Turn routine.

Since I generated these codes, I have worked out how to do a finish cut in the reverse direction.  My mistake was that I used a single combined roughing and finishing routine.  Next time, I will code separate routines for the roughing passes from right to left and the finish passes from left to right.  That will stop the big chip from being cut during the shoulder facing move as shown in my video here:

https://www.youtube.com/watch?v=Zxp-k4pQKTU

The threading is done with a hand coded G76 Mach3 routine.