Changing the Job / Material Size

[Tony Mac]

The material size for a job can be changed at any time by selecting,

Edit > Material Size

The Units, Width, Height, Thickness and Z Origin can all be changed on the form.

The origin for the job can be specified to be the bottom left corner or the middle of the job, and an offset distance can be entered to move the selected origin by the required X and Y distance.

Checking - Center vectors in material – will automatically reposition the vector design central to the new material size

Important – If the Z Origin is moved, all calculated Toolpaths MUST be recalculated.

We recommend that you recalculate toolpaths whenever the material has been changed.
This will ensure the toolpaths cut correctly on the CNC machine.

[Uncle Hai]

Hi Brian and Tony,
Thank you for your great job.
I have couple questions is crossing on my mind.
1/- How do you know where bit starts point, next and end of the project?
Can I fully control (demand) the section or line which will be first cut or next?
(I still use bottom left corner of material as my zero X, Y and Z Router home sitting
as the most)
2/- How do I understand single line to be carve if I want one long thin line?
Is double line a must for VCW?

I try to modify One of your BULLSHEAD sample.
Increase up the size to 48" long but I still want the whole concept.
When I try to create V-Carve toolpath, screen pop up to tell me
" The diameter of the selected tool is too small to fully machine the selected vectors.
The widest section of the selected vector is... 2.214 inches"
What is that mean?
I have to find the larger V bit's diameter or I have create more vector lines to meet the Demand?
The whole concept have to be change?
Would you please show me how!
Thanks,
Uncle Hai

[Tony Mac]

Hello Uncle Hai,

Good questions and perfectly timed.

1. When cutting around shapes the inside regions will always be cut first - ie the middle of a letter 'O' will be routed first.

2. Version 1.1 does only cut inside double lines. The New Version 2.0, which is about to be released includes new 2D Machining options that allow the cutter to Machine 'On / Inside / Outside' the selected vectors. These strategies can now be used with Ball Nose, Engraving, V-Bit and End Mill cutters and can machine at constant depth on or around the selected lines.

The 2D Machining also includes Pocket area clearance using an offset fill strategy
The cutting sequence can only be controlled by creating seperate toolpaths for each objects yo uwish to machine. If all objects are selected together, VCW will calculate an efficient path around each object.

3. Bulls Head example
Version 1.1 can only vcarve to the maximum depth calculated by the angle of the cutter and the widest region between the vectors in the design. So as you say, increasing the size of the job to 48" increases the gaps for the tool to cut, and the message states that a large tool is required.

Version 2.0 eliminates this problem, which is a BIG enhancement, allowing Small diameter tools to be used to vcarve wide areas by automatically calculating offset clearance passes in X & Y + multiple Z level passes if needed. The maximum Cut Depth can also be limited, allowing a Flat Bottom / pocket region can be routed using an End Mill, followed by the V-Bit to carve the detail.

This is easier to see in the images below than to explain.

The images show the Bulls Head scaled to 48" and carved to a depth of 0.75" using a 0.5" Dia End Mill for the flat regions and a 0.5" Dia 90 degree V-Bit for the detail / 3D Carving passes.

I am very confident that Version will now allow you to cut Large Designs using any size cutters - Version 1.1 needed lareg cutters for large jobs, which was often not pratical or impossible!

To show more clearly how the flat bottom machining works I have vcarved leaving the Bulls Head logo raised as this would require the tool to cut deeper in the wide regions.

Click on the images below to see more detailed pictures



I hope this answers your questions?

Tony

[Uncle Hai]

Hi Tony,
Thanks for quick respond but I still not clear about segment editing in question 1.
Is there any editing page somewhere in your software like Vector or Shopbot so I can PAUSE, ADD and CHANGE BITS etc..?
I really want total control about this (sorry I ask too much)
You guys really did awsome job to make this software more friendly use, so sign guy like me don't spend too much time strucgleling
in front of the computer to figue out how to accomplish the project to be due in next week
Can I purchase a software anytime even weekend?

Best Regards,
Uncle Hai

PS.
By the way,
I'd like to open VCarve software in full screen mode at every first time, any trick?
Thanks.

[Tony Mac]

VCW does not include manual start point control or toolpath ordering. This is because our development 'objective' is to provide a software solution that's quick to learn, easy to use and allows even the most novice of pc / machine users to succeed in machining very complex designs. Adding manual editing / control options etc. will result in the software becoming more technical and therefore more complex. If your work requires advanced level manual editing and control, I would suggest that you should look for an alternative solution.

I'll find out if the program can be opened in full-screen mode and let you know.

Our Secure On-Line payment methods can be used any time of the day or week. The Share-it link offers a fully automated method, supplying an immediate license code and instant access to download the full version of the software. The PayPal method is not automated and requires Vectric to issue the license and download details, which in some cases may take up to 12 hours.

Tony

[Scott]

Uncle Hai,

To get the program to open maximized each time you double click on the desktop icon, first right click on it and choose "Properties", then in the box next to "Run" click on the down arrow and choose "Maximize". Click "Apply" and "Ok" and you should be good to go. You can do this with the icon for Vcarve Wizard in your start menu and the quick launch menu if you have one there also.

Regards,
Scott

[Uncle Hai]

Thanks Scott and Tony.
You mention another alternative solution for manual editing and control,
you mean software can read script page?
Any suggetion?
Do I get version 2.0 if I purchase order now?
Uncle Hai

[Tony Mac]

Hi again,

If your work requires the ability to manually control start points & sequencing etc. then VCW is not the right solution.
You should consider buying some other package that offers such manual control, but I'm afraid we can't make any recommendations.

No, VCW does not read or run scripts or macros.

Yes, you would receive version 2.0.

Customers purchasing VCW automatically receive Free Upgrades to all new versions released in the next 12 months.

Tony

[Uncle Hai]

Thanks Tony,
Is 2.0 Trial Version available for download?

[Tony Mac]

We are very close to releasing verison 2.0 (customers have been testing V2 for 3 weeks), and should have a new downloadable Trial version available within the next 2 weeks.

Tony

[Uncle Hai]

Please drop me a note when you are ready.
Thanks a bunch
Uncle Hai

[RoutnAbout]

Why are we only allowed to use 50% or half the Tool Diameter when pocketing with an Endmill or Slotdrill. I've been known to use as much as 98% step over with a good sharp tool and have had good results.
Will this be a candidate for the wish list on future releases?


Don

[BrianM]

Hi Don,

The reason for limiting the stepover to half the diameter is to ensure that there are no 'upstands' left unmachined. Although for a rectangular pocket you could get away with almost 100% stepover, this is not the case for some irregular shaped pockets.

The image below shows the potential problem. The first stepover is the tool radius (obviously!), the second stepover is then 90% of the tool diameter. I have drawn the tool outline all along the offset passes to indicate the areas which would be machined by the tool. Where there is a sharp corner, an upstand would be left unmachined in the area I have coloured in red. This will not occur if the offset is restricted to half the tool diameter or less.

The next major release of VCarve Wizard will include the ability to clear areas using a raster pattern, and we will allow stepovers of upto the tool diameter for this strategy.

Hope this answers your question

Regards

Brian

[Paco]

Hi Brian!

May I suggest that this new raster area clearance strategie include a setting (or a default value) for when it's making the rastering clearance, it avoid going at the edge of the vector(s) bounderie(s) and then make a final cleaning outside pass following the vector(s) bounderie(s)?... the idea is to avoid any gouging of the vector(s) boundarie(s) while going back and forth. The other CAM that I use for this kind of routing leave thoses gouging (small but there) on the perpendicular sides of the raster moves of the area that's get cleared... even with the final outside pass of the area clearing toolpath. It may just need some 10% (may be better to be configurable for specific types of material; 0.03" can be OK in woods while it would be too much for metals) allowance to the vector(s) bounderies to avoid this while not changing much the machining process and the time involved. Let me know if I do not make sens and I will post a graphics...

As for the "Offset" area clear strategie (the current one in VCW), you might want to consider an "island re-machining" to remove thoses leftover... I know (think) there's more programming involved about this, but it would just benefit Vectric/VCW to do this. Offset area clear pocketting is my number one choice over raster clearing and I just need (wich) to be able to set the stepover like Don.

Still, keep up the good work fellows!

[RoutnAbout]

Thanks Brian,

Yes it does clear up my question. I Usually use a small hand chisel to clean those small areas up. I also like the fact that I don't have to with the less than 50% stepovers.

I also like the idea that Paco suggested about a clean up pass on the perimeter of a raster pocketing

Can't wait for the next release.
Keep up the great job

Don