[jmcglynn]

I'm using SolidCAM 2008 SP2.4 (the latest as of last week). I have a simple part that I need to thread mill, when I ran the generated program I got partial threads only on one side of the shoulder.

Looking at the g-code for the two operations that finish the OD of the boss that I want to thread, and the thread milling step I see something obviously wrong.

The boss should be at X1.75 Y-1.75. The operation that finishes the boss has its arc center at exactly that point.

The thread mill operation has the center off by roughly .012" on the y-axis (in different directions for the top arc and the bottom arc no less).

If you look at the screenshot in the backplotter you'll see what I mean.

Part accuracy is set to .0001 (default is .004)

Part of it at least seems to be the post, if I use the haas_3x_nosubs post that comes with solidcam it is only off by .003" and it generates a single move using IJ instead of two arcs using R.

Has anyone ever seen this?

Joe

[Brakeman Bob]

Joe, Have you told your reseller? I think they released R12 far too early and I have reported a number of bugs myself. As for thread milling, I program for Heidenhain code and my post is set up to generate threadmilling cycles from Drill jobs, so I never get to use the SolidCAM threadmilling option.

[jmcglynn]

Joe, Have you told your reseller? I think they released R12 far too early and I have reported a number of bugs myself. As for thread milling, I program for Heidenhain code and my post is set up to generate threadmilling cycles from Drill jobs, so I never get to use the SolidCAM threadmilling option.

Yes, I reported this to SolidCAM (I bought directly from them) and I'm working with tech support.

I have to agree on the bugs, although I saw a ton of problems in R11.2 and was told that they wouldn't fix them in R11.2 because it was "done" and R12 was coming out.

They are suggesting changing the post so that the thread mill moves use G03 with IJ instead of R. It seems to generate slightly more accurate code - but still not correct.

I had a problem with arc centers last summer and I just reproduced the problem in R12 - so I think that is where the issue is, not the post.

[jmcglynn]

I mentioned that I'd seen a similar bug where the arc centers are incorrectly calculated. I reproduced the bug and sent it to SolidCAM back in July and was told it was fixed. I just checked and it seems to still be there.

I made a simple part and set up two operations to cut the two shaped. When I check the arc center point for the large rounded end on both tool paths they are out by .006". The arcs should be concentric of course. This leaves a healthy step in a finished part and isn't acceptable.

Here is a screen shot from my backplotter and the part file (solidworks 2009 + solidcam 2008 R12 SP 2.4) The arc centers should be at X0 Y0, the selected one (in yellow) obviously isn't...

[Brakeman Bob]

Hi Joe. I tried to replicate your problem using a post for FANUC 16 that SolidCAM created for me back on V10 but I was unsuccessful (I think the post isn't all it should be on spiral milling).

However, the thought struck me that this might be a metric-to-inch thing. Have you tried doing the arc test in metric? I know that this doesn't help you much because you run your shop in inches, but it could supply a clue to SolidCAM where the problem lies and how to fix it.

If I get time later, I'll try the arctest in my heidenhain post using the SolidCAM threadmilling cycle and see what I get.

For info, I run SolidWorks 2008 SP4, SolidCAM R12 SP2.4

All the best

Bob

[BJ-DEKA]

Joe you mention changing the default tolerance from .004 to .0001. where was that tolerance? if it was the one in the cam part definition that is only for simulation... the tolerances you want to check are in the solidcam settings under units. there's is spline approximation and chain selection options. beyond that if there's still a problem i would say its a setting in the .mac or .gpp files.

hope this helps,
BJ

[jmcglynn]

Joe you mention changing the default tolerance from .004 to .0001. where was that tolerance? if it was the one in the cam part definition that is only for simulation... the tolerances you want to check are in the solidcam settings under units. there's is spline approximation and chain selection options. beyond that if there's still a problem i would say its a setting in the .mac or .gpp files.

hope this helps,
BJ

Just to close the loop on this, the solution I got back from SC was to change my mac file setting for ARC_QUADRANTS to Y. Setting it to N attempted swing the circle (360 degrees) in two arcs. When I checked the g code the arc centers were calculated wrong. This change made it behave properly...although this isn't a "fix" to my way of thinking, just avoiding the problem by forcing the software down a different path.