[loddie]

After reading most of the threads on this forum back to 2012, watching many of the MadCAM video tutorials, searching for solutions online, and studying the MadCAM help files, I’m struggling to setup a 4th axis with rotation limits (XYZA).

My set up is unique as the 4th axis has a bracket clamp to support the part (see attached image). Its ideal as it allows for machining concave regions on the bottom of the part without having to reorient it or use a 5 axis machine (which is not in the foreseeable future).

The disadvantage of the clamp design is possible tool crashes. My initial approach was to try limit the rotation angle of the 4th axis, an option in the Machine Setup. The clamp is positioned at 180 degrees (down, 6 o’clock, BDC) in the home position and requires about 40 degrees for tool clearance (+/-20º) at TDC. So if I could limit the tool paths to +/-160º, the clamp bracket won’t crash into the tool. Limiting the 4th axis angle in tool set up did not work in MadCAM 4.3 and does not appear to work in 5.0 trial version. I also tried setting up a 5 axis machine with the 5th axis locked (0º,0º) and the 4th axis angle limits set in both 4.3 and 5.0 with no luck.

Regardless of versions or settings, the generate tool paths in full 360º, resulting in tool crashes with the bracket clamp for both indexed and continuous 4th axis operations.

The attached tool path file is the best I can come up with after a several days of generating hundreds of tool path combinations (PM for tool path file as I can't seem to attach a Rhino file). Each part is custom and only machined once. The workflow I’ve come up with is less than desirable for one-off parts as each part/stock material is not always centered on the A axis. This requires tweaking every clipping plane (top and bottom) and boundary curves. The end result will work, except it probably takes five times longer than if the A axis rotation was limited and I could set up one finishing continuing finish pass instead on 5 indexed passes. I like to maximize set up efficiency itself of using the time consuming workflow I currently have.

FWIW, I’m using MadCAM trial version (5.0.2015.417) with the trial version of Rhino. I have Rhino 4 with MadCAM 4.3, but ran into the same 4th & 5th axis angle limitations (not functioning), so I thought I would try the trial versions of MadCAM and Rhino to verify it will work before upgrading two software packages for a singular application.

So this results in several questions:

1. Is the machine set up axis angle limitation designed to limited the rotation of the rotation axis as I envision it?
2. If it is, is it not functioning because it is a limitation of the trial version of MadCAM 5?
3. If not, any idea why I’m not able to set it up (I do save any settings changes)?
4. Are there other ways to limit the rotational travel of the 4th axis to prevent a tool crash with the clamp (eg, create a custom Drive Surface to prevent tool paths colliding with the bracket clamps)?
5. I’ve loaded .stl files of the bracket clamp into the machine setup. However, they do not appear in the simulations. This would greatly help visualize potential tool crashes. Is this a limitation of the 5.0 trial software?
6. Does anyone have tips for a better workflow than I’ve manage to scrape together?
7. In the Help file the clipping planes appear to be visible, likely so you can drag and drop them to raise and lower. However, the clipping planes don’t appear in any of the viewport windows. Is this typical?
8. Regardless of whether the stock material layer is visible (or not) and the simulator settings, the simulator does not show the removal of stock material, only the part is shown (see attached image). This makes it difficult to set Clipping Planes, etc. for subsequent finish passes. Is this a limitation of the trial version?

One observation that may help others with setting up a 4th axis: When setting up the Boundary Curves, I found them to only effective if drawn in the X plane (front/back viewport). I found this out by accident after several hours of trying to configure BCs in the Z plane. The Region curves are effective if drawn in the Z plane. This seems odd as both are effective in the same plane (Z), yet are drawn in different planes. Perhaps it is only the version of the software I have.

I’ve reached out to the MadCAM support, but as I haven’t received a response, I guessing JM is enjoying summer sailing. So if any seasoned MadCAM users have answers and/or would be willing to review the attached file(s) and suggest ways to improve the current workflow, your help would be most appreciated. Also, I realize what I am trying to accomplish may be outside the design intentions of the MadCAM software, and some the preceding limitations may be due to the trial version of the software.

Thank-you,

LO

[loddie]

In case anyone else is experience similar problems or looking for solutions, here are some answers:

1. Seems as though the software is capable of rotary axis limits. However, the following thread suggests a "custom dll" must be written or the feature is not functional as intended: http://www.cnczone.com/forums/showth...ation%20limits
Unfortunately I cannot find info on creating a "custom .dll". It appears "External DLL support for machine kinematics" are only available as an option for the 5Xtra version (out of my budget): http://madcamcnc.com/features/

2. According to the developer, the demo version works as a full version: http://www.cnczone.com/forums/madcam...am-5-axis.html. Thus, this problem appears to not be a limitation of the trial version.

3. See 1&2 above. Appears to be a software limitation.

4. A drive surface may work. Will have to experiment. However, drive surface options are limited to the 5Xtra, which is out of my budget.

5. See 2 above. The trial version = full version. As I had other problems with the simulation, I purchased and installed a replacement graphics card with support for OpenGL (Nvidia Quadro 600). This resulted in significant improvement of the simulator (at least three times faster, subjectively). However, installing an OpenGL graphics card did not result in the simulator showing the machine parts or material stock removal.

6. Apparently not...although this thread only has had 140 views and is only a week old...:

7. Perhaps related to video card issue (see 5 above). Will try tomorrow.

8. Apparently not supported in 4th and 5th axis simulations: http://www.cnczone.com/forums/archiv.../t-274726.html & http://www.cnczone.com/forums/madcam...simulator.html

I haven't yet figured out a suitable workflow, but am hopeful to soon. Been doing doing lots of experimenting. MadCAM seems very promising and capable, although support seems to require much patience.

[svenakela]

You can't expect a lot of support on a free demo download, unfortunately.
As you've already found out the 4/5 axis will not show material removal. I think that's a major feature in a coming release, but I don't know when.

I don't have madcam in front of me, but isn't there an angle limit in the machine setup?

[loddie]

Svenakela, thank-you for your blog and videos! I've watched all of them and some repeatedly. It was your 4th axis indexed video that helped me come up with a suitable solution.

Yes, there is an angle limit in the machine setup. But it has no effect for me. Tried many different angles, 4 & 5 axis set ups, and +/-degree combinations.

So I finally came up with a suitable workflow today. Roughing at +/-90deg, setting the bottom clipping planes to zero. Then planar finishing at 135, 45, -45 and -135 degrees, using both clipping planes and region curves to restrict the tool path. All region curves were 5 sided polygons to keep the cutter away from the clamps and were drawn on the Z plane. There is some repeated machining with this workflow, but it isn't too bad and the clamps are safely out of the way of the cutter.

In my version of MadCAM, the remachining selections don't have options for stopping at the part line. Thus, the remachining tool paths aren't a great option. I'll keep experimenting. After a week of this full time, I'm starting to feel proficient.

Unfortunately my demo of MadCAM 5 does't have any post processors. I tried using post processors from MadCAM 4, but the A axis never moves from home in the G code file. So I'm unlearning MadCAM 5 and downgrading back to MadCAM 4 as those post processors do seem to work with the A axis. Hopefully will cut the real thing soon after I resolve other minor set up issues. Mike is trying to find a post processor for MadCAM 5 for me to try (I have EdingCNC control which follows the NIST RS274/NGC standard) as my preference is to upgrade. However, as both my wife and I are temporarily unemployed, I want to be sure he Rhino 5/MadCAM 5 combination works with my machine before spending $$$$ to upgrade.

[loddie]

In the Help file the clipping planes appear to be visible, likely so you can drag and drop them to raise and lower. However, the clipping planes don’t appear in any of the viewport windows.

After installing an OpenGL video card and updating the drivers, I'm still not able to view the clipping planes. However, it is a non-issue as I used to using the clipping plane dialogue box instead.

[Gregore]

I use the same kind of custom jig you use , and I know angle limits can be set via drive surface .

Your trial version should have come with the post processors so you might want to try down loading again , if that does not work you can copy the post processor from madcam 4 and use it in madcam 5 .

If the Gcode post is still not limiting the 4 th axis after you sent limits in the machine set up I would guess that it could be the post you are using

I am away until Monday later in the day and can look at that time if the limits are working on my post

[svenakela]

Can you make a screen shot of the GUI when you have the clipping planes activated?
Actually I haven't tried moving them when setup, I always use the dialog. But still they should be visible.

I'll see if I can dig into the angle limit problem this weekend.

[Dan B]

Do you have any samples of how your code should look for that controller? If so, I could probably write a post for you. I already have a 4-axis post for one of our machines down in the US. It shouldn't be that difficult to adapt it to the syntax your machine requires.

Dan

[Gregore]

I think a better way than clipping planes to handle the control of where the cutter does not go is in 3 axis cutting tools via the tool called "with in boundary curves "
You can rotate the model to the angle you want then select it as current model , then create line around area you wish to cut inside ( you could also fill inside the line with a plane and move this plane up and down to control the depth of cut ) when you wish to do another area you tilt model around 0,0,0 and reselect as new model .

I do it this way a lot on a 180 flip cut and also when I want to cut only a small controlled area at an angle other than 0 or 180

A lot of the cutting I do is in wax with small tabs to hold the part as everything is cut away around it and this allows madcam to not cut the tabs free from the material

[loddie]

I use the same kind of custom jig you use , and I know angle limits can be set via drive surface .

This is good news. I'll revisit drive surfaces today.

Your trial version should have come with the post processors so you might want to try down loading again , if that does not work you can copy the post processor from madcam 4 and use it in madcam 5 .

Good idea. I uninstalled MadCAM and tried reinstalling MadCAM 32 & 64 bit versions, but neither had any post processors. I searched the program folders as well.

From what I can gather online, LinuxCNC (EMC2) following the same NIST RS274/NGC standard as my EdingCNC controller. I think it is also very similar to Fanuc. So I tried several MadCAM 4 post processors in MadCAM 5. The Fanuc and generic AXYZ did not generate any A axis G codes. The EMC2 4 axis process shows the A axis in the post file. However, the indexed moves seen in the simulator (90, -90, -135, -45, 45, & 90) are not processed. Every A axis position in the post is 0 degrees.

I am away until Monday later in the day and can look at that time if the limits are working on my post

Much appreciated!

[loddie]

Svenakela, after reinstalling MadCAM 5 at Gregore's suggestion, I can now see the clipping planes and move them with the gumboil. So this problem is resolved. Thank-you for being willing to check it out.

[loddie]

Do you have any samples of how your code should look for that controller?

Dan, the attached file is a post processor developed for the EdingCNC for Fusion360. Originally, I was going to use Fusion360 CAM, but it does't not appear to be capable of generating tool paths from scanned quad/triangulated meshes. So I never even got to the point of testing this post processor with Fusion360 on my machine.

If so, I could probably write a post for you. I already have a 4-axis post for one of our machines down in the US. It shouldn't be that difficult to adapt it to the syntax your machine requires.

Much appreciated. I didn't think it was difficult and probably can be done in less than five minutes. Unfortunately, I lack the knowledge to do so.

[loddie]

I think a better way than clipping planes to handle the control of where the cutter does not go is in 3 axis cutting tools via the tool called "with in boundary curves "

Gregory, I just use the clipping planes to control the depth of cut. I've been using region curves to control where the cutter goes. The simplified workflow that works in MadCAM 4 is:

1. Roughing passes @90deg and -90deg. Set clipping planes to control depth of cut. Set region curves to control where cutter goes.
2. Finishing passes @-135, -45, 45, and 135deg. Set clipping planes to control depth of cut. Set region curves to control where cutter goes.

I'm only using clipping planes to because my Z travel in limited to 7". These has created a new problem where tool paths created in Z are exceeding the limits of the machine, see new thread: http://www.cnczone.com/forums/madcam...ml#post1893292

create line around area you wish to cut inside ( you could also fill inside the line with a plane and move this plane up and down to control the depth of cut )

Great tip! I didn't realize you could set depth with the region curves with a plane. I try to do that today.

A lot of the cutting I do is in wax with small tabs to hold the part as everything is cut away around it and this allows madcam to not cut the tabs free from the material

To protect the workpiece clamps, I created an oversized shell over them, that way if I wasn't perfect with the region curves, the tool cutter will not crash into the real clamps.

[loddie]

Can you make a screen shot of the GUI when you have the clipping planes activated?
Actually I haven't tried moving them when setup, I always use the dialog. But still they should be visible.

I'll see if I can dig into the angle limit problem this weekend.

That would be great! The workflow I've come up with in MadCAM 4 could be improved.

I'm hoping that if the rotation limits can be set in MadCAM, then hopefully only two tool paths will be needed: one continuous rotational roughing and one continuous rotational finishing. Here is the end goal: https://www.youtube.com/watch?v=_jTp...siA1P&index=59


After dozens of times setting up the tool paths, I managed to reduced the time from opening MadCAM to importing into the CNC machine software to about 30 minutes. This is using templates with region curves, etc. Unfortunately, I also have to edit the post G code file the correct A axis positions and manually limit many Z axis clearance tool paths. If this was for making dozens, hundreds, or thousands of parts, no big deal. But as creating tool paths is only one step in the process for a quantity of one, it would be nice to minimize processing time.

FWIW, I'm scanning the lasts and only importing them into Rhino/MadCAM to duplicate them. I'm not reshaping them or changing them. Unless I can improve the entire digital workflow (scanning, aligning, tool paths, post process, etc.), it would be just as fast to use a manual router duplicator.

[Gregore]

Yes you can use region curve to cut only inside of a controlled area and if you use the same line to first make a plane and move it to the level you want the cutter to stop at it will work fine , but you have to first select it as part of the model.

But also when it is no longer needed you have to remember to select the model with out it.

[svenakela]

I put some time into this over a breakfast coffee and these are my ideas so far.
The angle limits in the machine setup is only to tell the tool path generator how far you can go before it's time to revolve and continue from the other side. The optimal solution for you would be 5xtra and Drive Surface. That would cover you entirely. You gotta sell some more shoes a week or two and you have covered the cost.
But if you want to stay with 4 axis you should be able to do it with a Region Curve. You could probably keep one region curve as a template together with your fixture and reuse it all the time.

Here are a few examples of 4 axis paths with a region curve. If you tweak it a little bit you should be able to come close to a faster solution than the one you are doing now.


Attachment 322390

[loddie]

I put some time into this over a breakfast coffee and these are my ideas so far.

Svenakela, thanks for looking into it!

The angle limits in the machine setup is only to tell the tool path generator how far you can go before it's time to revolve and continue from the other side.

This is what I thought. I can easily set the A rotary axis limits in the EdingCNC software setup to prevent crashing into the bracket clamps. I was hoping the axis angle limits would function similarly in MadCAM. However, they seem to have no effect on the tool path. Here is a screenshot with a 4 axis machine setup with angle limits at -160deg and 160deg on A axis. It may not be obvious from image, but the tool paths revolve through all 360 degrees. On the machine this will result in tool crashes with the bracket clamp as the Z axis does not have enough travel to clear the clamp bracket (Actually, the EdingCNC software won't allow the file to started as it knows the rotary angle limits are exceeded). The lack of rotary axis rotation limits is the main problem I was hoping to resolve with this thread.

Attachment 322506

The optimal solution for you would be 5xtra and Drive Surface. That would cover you entirely

I tried playing with the Drive Surface today. As this is a scanned object (.obj or .stl file), I don't think it is the correct type of object for a Drive Surface. Whether I selected the shoe last first or the Drive Surface option first, I could not chose the foot last as a drive surface. Probably because it is a mesh, not a NURBS or T-Spline. I had a similar problem in Fusion360 which requires the mesh to be reverse engineered to a NURBS or T-Spline before a tool path could be created. Reverse engineering is a time consuming process and the reason I gave up on Fusion360 and came back to MadCAM.

But if you want to stay with 4 axis you should be able to do it with a Region Curve. You could probably keep one region curve as a template together with your fixture and reuse it all the time.

This is the best approach I been able to accomplish so far. I really like the region curves you created. I didn't realize region curves didn't have to be confined to a single plane, so I created a region curve inspired by your design and added it to the template collection. Unfortunately, the axis limits described through this thread remains a problem. And I agree, if the axis limits are resolved and I use a cylindrical region curve for one continuous roughing and one continuous finishing planar pass, the processing time will drop to a only 10 minutes! For the indexing workflow, I've already setup templates, and after practicing a couple dozen times, the fastest I could load tool paths in the EdingCNC controller is 30 minutes.

[sathishs]

nice post to read

NCCS has built its reputation and business by providing an outstanding service, comprehensive knowledge and superior quality products at affordable prices.

We have a wide range of customers throughout Australia and offer solutions to program most of the CNC machines including Milling, Turning, EDM, Plasma, Laser, Punch and powerful communication software for CNC controllers.

Now to add we have been chosen as a Value Added reseller for the world’s No13D CAD
For more details:www.nccs.com.au

[svenakela]

...

I tried playing with the Drive Surface today. As this is a scanned object (.obj or .stl file), I don't think it is the correct type of object for a Drive Surface. Whether I selected the shoe last first or the Drive Surface option first, I could not chose the foot last as a drive surface. Probably because it is a mesh, not a NURBS or T-Spline. I had a similar problem in Fusion360 which requires the mesh to be reverse engineered to a NURBS or T-Spline before a tool path could be created. Reverse engineering is a time consuming process and the reason I gave up on Fusion360 and came back to MadCAM.

...

This is the best approach I been able to accomplish so far. I really like the region curves you created. I didn't realize region curves didn't have to be confined to a single plane, so I created a region curve inspired by your design and added it to the template collection. Unfortunately, the axis limits described through this thread remains a problem. And I agree, if the axis limits are resolved and I use a cylindrical region curve for one continuous roughing and one continuous finishing planar pass, the processing time will drop to a only 10 minutes! For the indexing workflow, I've already setup templates, and after practicing a couple dozen times, the fastest I could load tool paths in the EdingCNC controller is 30 minutes.

You can add another surface on top of your model as a drive surface, that's the beauty of the Drive Surface command. Also, the tool will be perpendicular to the drive surface which means that you can make the cutter to go into the model with an angle if necessary (like going "behind" tabs etc). With a drive surface as a part of your template you would be able to do this in minutes.

I've been talking about a angle limiting feature with JOM earlier to make it easier to setup an angle limit. I hope it will come in a future release.

[Gregore]

I do not understand why angle limits are working for svenakela but not for loddie , both of your images are just screen captures of tool paths something has to be wrong with loddies set up either in machine set up or the post processor .

Also very cool svenakela ..... I did not know you could use region curves in a rotary cut , it looks like it works just like a drive surface